A P P N O T E S. Abstract... 4 Chapter 1: Setting up the Design Data Exercise 1: Overview... 5

Transcription

1 AppNote MG A P P N O T E S SM DxDesigner Tutorial for the Expedition PCB Flow By: DxDesigner Customer Support Last Modified: August 15, 2012 Valid Software Versions: EE Table of Contents Abstract... 4 Chapter 1: Setting up the Design Data... 5 Exercise 1: Overview... 5 Prerequisites... 5 Design Data Overview... 6 Checking For Pre-Existing DxWDIR Folder... 6 Backup Pre-existing DxWDIR Folder... 7 Copy DxWDIR Tutorial Data to Local Location... 7 Get Design Data from SupportNet... 7 Exercise 2: Setting the WDIR and DxTutorial Variables... 8 Exercise 3: Setting Up DxDataBook... 9 Exercise 4: Opening a Project Exercise 5: Project and User Settings Project Settings User Settings Set Up Units and the Grid Set Up the DxDesigner Navigator Set Up Default Sheet Size Set Up Rules for Copying Chapter 2: Navigating in DxDesigner Exercise 1: Navigator Tree Pane August 15, 2012 Page 1 of 207

2 DxDesigner Tutorial for the Expedition Enterprise Flow Exercise 2: Zooming Exercise 3: Help System Exercise 4: Window Tabs Feature Exercise 5: Thumbnail Viewer Exercise 6: Find/Replace Function Exercise 7: Properties Pane and ICT Viewer Chapter 3: DxDesigner - Selecting and Verifying Parts with DxDataBook Exercise 1: Configure DxDataBook Exercise 2: DxDataBook Libraries Exercise 3: Component Selection with DxDataBook Chapter 4: DxDesigner Schematic Manipulation Exercise 1: Creating a New Schematic Exercise 2: Adding a Sheet Border Exercise 3: Adding Components Exercise 4: Adding Power and Ground Connections Exercise 5: Moving Components Exercise 6: Connecting the Components with Nets Connecting by Abutment Creating Nets Using the Right Mouse Button Creating Nets using Net Mode Exercise 7: Naming Nets Adding Names using the Navigator Exercise 8: Modifying Properties Property Visibility Modifying Property Values Adding New Properties Exercise 9: Working with Busses Exercise 10: Copying Symbols Exercise 11: Renaming Properties Exercise 12: Completing the Channel Circuits Exercise 13: Using Arrays Chapter 5: DxDesigner Hierarchical Design Exercise 1: Preparing for Hierarchical Design Exercise 2: Bottom-Up Hierarchical Design August 15, 2012 Page 2 of 207

3 DxDesigner Tutorial for the Expedition Enterprise Flow Exercise 3: Using a Hierarchical Block Exercise 4: Top-Down Hierarchical Design Chapter 6: Constraint Definition with CES Exercise 1: Navigating CES Exercise 2: Assigning Constraints and Understanding Constraint Class Hierarchies Exercise 3: Creating Constraint Classes Exercise 4: Net Classes and Schemes Chapter 7: Preparing a Schematic for PCB Design Exercise 1: DxDesigner Diagnostics Exercise 2: Hierarchical Verification with DxDataBook Exercise 3: Design Rule Checks with Tools > Verify Exercise 4: Packager Exercise 5: Expedition PCB Exercise 6: eexp View Chapter 8: Documenting DxDesigner Schematics Exercise 1: Cross Referencing Cross Reference Settings Exercise 2: DxPDF Exercise 3: Partlister Exercise 4: Archiving Projects August 15, 2012 Page 3 of 207

4 DxDesigner Tutorial for the Expedition Enterprise Flow Abstract This AppNote is a tutorial for the EE release of DxDesigner. The primary focus is on schematic capture with DxDesigner, including DxDataBook. CES, Expedition PCB, and supporting utilities are also briefly covered by this tutorial. The goal of the tutorial is to introduce new users to fundamental concepts and techniques to successfully create schematics using DxDesigner. You should allow for approximately 12 hours to complete this tutorial. A video showing updates to the user interface for EE release can be seen here: Video: DxDesigner EE7.9.4 Release Highlights (10 min). For instructor-led training on DxDesigner and other Mentor Graphics products, please consider attending Mentor Graphics training classes from Mentor Graphics Education Services department. Additional AppNotes, TechNotes, movies, and documentation can be found on SupportNet. August 15, 2012 Page 4 of 207

5 DxDesigner Tutorial for the Expedition Enterprise Flow Chapter 1: Setting up the Design Data Welcome to the DxDesigner Tutorial for the Expedition Enterprise Flow! This tutorial walks a person through the basic flow through the DxDesigner toolset in the Expedition PCB flow using a moderately complex circuit. Over the course of this tutorial, you will learn the following: Navigating in a DxDesigner schematic Selecting and verifying parts using DxDataBook Creating schematics with DxDesigner Creating hierarchical schematics with DxDesigner Using CES to add constraints to your board Forward annotating your schematic for Expedition PCB Using utilities to document your DxDesigner schematic As a primer for this tutorial, the following short video will follow the creation of a simple design in DxDesigner: Video: Small Amplifier Design Lab (13 min). This video is part of a larger video series that contains content that is beyond this scope of this tutorial. Also this video series was made for the DxDesigner release, but is still applicable for the release. The full series of videos can be found here: DxDesigner for University Video Series (1hr 15min). Exercise 1: Overview The tutorial assumes no prior knowledge of the tools, just a familiarity with schematic capture and layout environments. The tutorial is organized in the same way that you would create a real design. You begin by setting up the DxDesigner environment, you proceed to draw a schematic, run reports, run a simulation and pass the design to Expedition PCB for layout. The design you create in the early topics will continue to be used as you perform more advanced tasks. Prerequisites Your Operating system is Windows. This tutorial is currently not supported on UNIX or Linux. Installed DxDesigner (version EE 7.9.4) Installed DxDataBook Installed CES August 15, 2012 Page 5 of 207

6 DxDesigner Tutorial for the Expedition Enterprise Flow Installed Expedition PCB Design Data Overview The DxDesigner tutorial data can be found in a downloadable DxTUT.zip file from SupportNet. See the following figure for the structure of the.zip file. Note: Instructions on how to download the files and where to extract them can be found on page 7-8. \DxWDIR \DxTUTORIAL \templates \DxConfig \DxTUT_Lib \DxTUT_Proj \DxTUT_Sample A brief overview of the tutorial and tutorial data located in the DxWDIR folder is as follows: DxTUTORIAL - Contains data for this tutorial covering a real-world design example DxTUT_Sample - Contains DxTUTORIAL design data in various stages of completion DxConfig - Contains ancillary files used in some topics DxTUT_Lib - Contains a Central Library templates - Template files are located in templates\dxdesigner\expedition DxTUT_template.prj Checking For Pre-Existing DxWDIR Folder You need to check for a pre-existing DxWDIR folder to avoid losing data. If your local WDIR variable currently points to a folder with the name DxWDIR and location where you want to place the examples data, you need to back it up before starting, as the examples data will take precedence over your existing configuration. The DxDesigner tutorial and the tutorial August 15, 2012 Page 6 of 207

7 DxDesigner Tutorial for the Expedition Enterprise Flow designs expect your WDIR variable to be set to the DxWDIR folder provided with this tutorial, after you copy it into to your file system. Note: If your WDIR is currently set to your working environment location, you should note the current WDIR setting so you can later restore it to the original value. To check where your current WDIR variable is pointing, do the following: 1. From your Windows XP system Start menu, choose Control Panel > System > Advanced (tab) > Environment Variables (button) to access the Environment Variables dialog. a. Note: The Windows 7 path is similar at: Start menu > Control Panel > System (link) > Advanced system settings (link) > Advanced (tab) > Environment Variables (button). 2. In the System variables section, locate the WDIR item and click the Edit button. The Edit System Variable dialog appears. a. If the WDIR variable points to a folder called DxWDIR in the same location where you want to copy this tutorial DxWDIR folder, you should back up your original DxWDIR folder as described in the topic Backup Pre-existing DxWDIR Folder. b. Otherwise you can skip to the Copy DxWDIR Tutorial Data to Local Location topic. 3. Cancel the Environment Variables and System Properties dialogs. Backup Pre-existing DxWDIR Folder These steps only apply if your local WDIR variable points to an existing folder called DxWDIR that is located in the same location that you want to install the DxWDIR folder that comes with the DxExamples: 1. Before running the tutorial, create a backup of your existing configuration by saving your local DxWDIR folder to a different location. 2. When you have completed the tutorial, replace the tutorial DxWDIR folder with the backed-up version of your own DWDIR folder if it makes sense to do so. Copy DxWDIR Tutorial Data to Local Location You can download the design data from SupportNet. You should copy the DxWDIR folder to a local writable location, such as your C: drive as described below. Get Design Data from SupportNet August 15, 2012 Page 7 of 207

8 DxDesigner Tutorial for the Expedition Enterprise Flow This section assumes that you are getting the DxWDIR folder from DxWDIR_EE7.9.4.zip from SupportNet. 1. Download the DxDesigner tutorial data. 2. Unzip the file DxTUT.zip anywhere in your file system. Make sure you have at least 400 MB of free space. Note: In the resultant directory there is a.\dxwdir tree. This is where the tutorial data is located. Exercise 2: Setting the WDIR and DxTutorial Variables The WDIR environment variable is used by DxDesigner to locate default templates, software executables, and project files. The DxTUTORIAL variable is used during the project setup to specify the location of the Central Library to avoid hard-coding this path in the project. 1. Change the WDIR environment variable to point to the DxWDIR folder as follows: a. From your Windows system Start menu, choose Settings > Control Panel > System > Advanced (tab) > Environment Variables (button) to access the Environment Variables dialog. Note: The Windows 7 path is similar at: Start menu > Control Panel > System (link) > Advanced system settings (link) > Advanced (tab) > Environment Variables (button) b. In the System variables section, locate the WDIR item and click the Edit button. The Edit System Variable dialog appears. c. Set the WDIR path so {your_path}\dxwdir is at the front of the path, similar to that shown below and click OK: August 15, 2012 Page 8 of 207

9 DxDesigner Tutorial for the Expedition Enterprise Flow NOTE: This is a good opportunity to make sure that the WDIR variable points to the correct software installation tree! 2. Create a user variable called DxTUTORIAL to point to the DxTUTORIAL folder as follows: a. From the Environment Variables dialog, in the User variables section, click the New button. b. In the Edit User Variable dialog, create the DxTUTORIAL variable so that it points to the {path_to_dxwdir}\dxtutorial folder, similar to the following example: c. Click OK. d. In the Environment Variables dialog, click OK. e. In the System Properties dialog, click OK. Exercise 3: Setting Up DxDataBook Most of the part instantiations for the tutorial design will be performed from an application called DxDataBook. DxDataBook uses an ODBC (Open DataBase Connectivity) connection to link to any ODBC compliant database (for example, MS Access, MySQL, Oracle, etc.). In order to use DxDataBook, a new ODBC DSN (Data Source Name) must be created to point to the tutorial Access database as follows: 1. Ensure that DxDesigner is closed. 2. If you are using the Windows 7 operating system launch the ODBC Data Source Administrator program by double-clicking odbcad32.exe at C:\Windows\SysWOW64. August 15, 2012 Page 9 of 207

10 3. If you are using Windows XP open the Start menu and choose Settings > Control Panel > Administrative Tools > Data Sources (ODBC) to bring up the ODBC Data Source Administrator. The SampleLib DSN will be created for this tutorial. 4. Select the User DSN tab and click the Add button to add a new User DSN. 5. In the Create New Data Source dialog box, choose the Microsoft Access Driver (*.mdb) driver and click Finish. The ODBC Microsoft Access Setup dialog appears. 6. In the Data Source Name field, enter SampleLib. Note: The Data Source Name is case-sensitive, so make sure you follow the text case as shown above. 7. In the Description field, enter: DxDataBook for Tutorial. 8. In the Database section, click the Select button. August 15, 2012 Page 10 of 207

11 9. In the Select Database dialog, browse to the sdd_demo.mdb database located at C:\DxWDIR\DxTUTORIAL\DxTUT_Lib\sdd_demo.mdb as shown below. Note: The above file path assumes you have installed the DxWDIR folder in your C: drive. 10. Click OK in the open dialog boxes. DxDataBook is now configured for your machine. Exercise 4: Opening a Project To build a schematic in DxDesigner, you must first create a project. A project is a directory of folders and files that store the relevant details of the schematic, log files, part lists, and, even the PCB layout. DxDesigner must open the project file (.prj) in order to start your schematic design session. Projects can be opened using the Dashboard application (Start > All Programs > Mentor Graphics SDD > Dashboard) or by selecting the project file (.prj) in Windows Explorer. In the steps below you will use Windows Explorer to open the tutorial project. 1. In Windows Explorer, navigate to ${DxTUTORIAL}\DxTUT_Proj. August 15, 2012 Page 11 of 207

12 DxDesigner Tutorial for the Expedition Enterprise Flow 2. Right-click DxTutorial.prj and choose Open With > DxDesigner Application. This will open the tutorial project in DxDesigner. Note: If DxDesigner is not set as the default application for a.prj file, you can rightclick on the.prj file and choose Properties to specify DxDesigner as the application that will open.prj files. If you do this, you will be able to simply double-click the project file to launch DxDesigner. Exercise 5: Project and User Settings This section describes settings you can change in DxDesigner and differentiates the Project Settings that are stored in the project file (.prj file) and the User Settings that are stored in the DxDesigner.xml file. The former viewdraw.ini file is no longer used to store settings. The project file is located in the root directory of the project (in this tutorial, ${DxTUTORIAL}\DxTUT_Proj\DxTutorial.prj). The DxDesigner.xml file is located in the WDIR folder. The DxDesigner.xml file can reside in any, some, or all of the directories referenced by the WDIR environment variable. If a setting appears in two or more of the DxDesigner.xml files, the setting in the highest level the leftmost directory as it is displayed by the WDIR environment variable will take precedence. Project Settings This section provides an overview of the Project settings. No additional project settings are changed in this section. The project settings will typically apply to all of the projects and generally should not be changed by users. Key Project Settings can be set in a pre-defined template that is selected when the user creates new projects. Templates are also a good way to ensure that DxDesigner s settings are consistent among users in a design group. August 15, 2012 Page 12 of 207

13 DxDesigner Tutorial for the Expedition Enterprise Flow The Settings dialog page that you open through the Setup > Settings menu in DxDesigner makes it very easy to understand what belongs to the project settings or to the user settings as shown below. In the sections that follow, DO NOT CHANGE settings randomly. Only change the settings detailed in the instructions below. Changing settings that are not covered in the tutorial instructions could cause DxDesigner to behave differently and lead to deviations in the results that you produce. August 15, 2012 Page 13 of 207

14 Project settings are organized into the following sections: Special Components: Defines the path to the speccomps.ini file containing predefined symbol names for hierarchical ports based on the pin type (Input, output, bidirectional, tri-state, open collector, open emitter, analog, power and ground), for on/off-sheet connectors and for power/ground. Bus Contents: Defines the path to the busconts.ini file containing predefined bus names (typically standard buses or in-house buses) which are available to the users in the editors. Borders and Zones: Defines the path to the border.ini file containing predefined symbol names for various border sheet sizes (A0 A4, A E sheet sizes). Borders can be automatically inserted while creating a new sheet. These settings are stored in the borders.ini file. Also defined here are zone settings. For more information, see the following documents: o Partitioning a Sheet into Zones in the DxDesigner User s Guide o Displaying Sheet Border Zones in the DxDesigner User s Guide o Setting Zones to Match an Existing Border Symbol in the DxDesigner User s Guide Cross Reference: Defines how the link annotations appear on the schematic. This method was introduced in EE and will eventually replace the Tools > Cross Reference method of creating cross references on links (such as off-sheet and onsheet references). Net Name Delimiter: Useful to manage bus range values such as ADDR(7:0). None, curly brackets ( ) or square brackets [ ] are supported. DxDataBook: Points to a DxDataBook configuration file (.dbc) which is explained further in Chapter 3 of this tutorial. Sheet Numbering: Specifies which sheet numbering scheme is used. Export HDL: You specify the VHDL or Verilog parameters of a design. This tutorial does not cover this topic. You can enter project settings by way of the graphical user interface if needed. In general, they are pre-defined in a Template accessible from the project Creation dialog page. More information can be found in the Creating a Template File topic in the DxDesigner Administrator s Guide. Template files and project files share the same syntax which makes it easy to create a Template project. August 15, 2012 Page 14 of 207

15 DxDesigner Tutorial for the Expedition Enterprise Flow A portion of the template used in this tutorial (${DxTUTORIAL}\templates\dxdesigner\expedition\Tutorial.prj) is shown as follows: SECTION DesignInfo KEY BorderSymbols "${DxTUTORIAL}\DxConfig\borders.ini" KEY Bus_Contents "${DxTUTORIAL}\DxConfig\busconts.ini" KEY CentralLibrary "${DxTUTORIAL}\DxTUT_Lib\Master.lmc" KEY DBCFile "${DxTUTORIAL}\DxTUT_Lib\SampleLib.dbc" KEY DxD_Version "7.9.2" KEY FrontEndSnapshot "DxD" KEY HdlUtilsConfigFile "hdlutils.ini" KEY NetNameDelimiter "()" KEY PinComponents "${DxTUTORIAL}\DxConfig\speccomp.ini" KEY SheetsEditMode "1" ENDSECTION You can click on the different items of the Project Settings dialog page to see what the user interface looks like. You will change a few of these settings in the following sections of this chapter. User Settings User settings are defined from the DxDesigner Setup > Settings menu. User settings are divided into the following major categories, some of which are further divided into subcategories. We will only change a few of them in the next sections. Schematic Editor: The Schematic editor section includes options such as Units, Grid, and the New Sheets definitions. Graphical Rules Checker: Options for the setting reporting of graphical rule violations. Interconnectivity Table: Options for the ICT Viewer and the InterConnectivity Editor (ICE). ICE is not covered in this tutorial. The ICT Viewer will be described in Chapter 2. Navigator: The Project Navigator section controls the format of items displayed in the Navigator Window. Display: Controls the color various objects and fonts for the Graphic area of DxDesigner. DxDesigner Diagnostics: Controls whether Tools -> DxDesigner Diagnostics is run when exiting DxDesigner. August 15, 2012 Page 15 of 207

16 DxDesigner Tutorial for the Expedition Enterprise Flow Cross Probing: Controls cross probing options between DxDesigner and the chosen layout system. Sheet/ICT Backup: Controls behavior of automatic sheet/ict backups. Project Backup: Controls project's backups and backup settings. HDL/FPGA Integration: Control HDL simulation parameters. Run on Startup: Specify Forms or Scripts that will run when DxDesigner is started. DxDataBook Data Source: Allows the user to enter a user name and password for a DxDataBook data source. Licensing: Controls which licenses you check out. Advanced: Contains various optional settings for DxDesigner. In the User Settings section of the tutorial you change a few settings: Units DxDesigner Navigator Default Sheet Size Rules for Copying Set Up Units and the Grid Set the units to Inches as follows: 1. In DxDesigner, select Setup > Settings > Schematic Editor. 2. Make sure that the Unit is set to inches. 3. Verify that the Display Grid box is checked and the Grid Spacing is set to 0.1 in. The default Grid Type is Lined as shown in this tutorial, but can also be changed to Dotted. August 15, 2012 Page 16 of 207

17 DxDesigner Tutorial for the Expedition Enterprise Flow 4. Verify that the Grid Interval Markings box is checked. 5. If you had to change any setting, click the Apply button. The Settings dialog box does not close with the Apply button. We will continue to use this dialog in the next section. Clicking OK closes the dialog. If your settings are different than the defaults, clicking the Apply (or OK) button writes those settings in <WDIR>\DxDesigner.xml. Only settings that differ from the default settings are stored in that file. From now on, all the dimensions in all the dialogs are expressed in inches. Set Up the DxDesigner Navigator DxDesigner s Navigator can be configured to display net, symbol, and block information in a variety of formats. In the following steps you will configure the format of Info Tips for symbols. 1. From the Setup > Settings dialog, select Navigator > Symbols. 2. In the Symbols section of the Settings dialog, click the icon on the right side of the Info Tip format option and select Property: Ref Designator. August 15, 2012 Page 17 of 207

18 3. In the Info Tip format dialog, add > characters as shown below. This will improve the readability of the Info Tip. 4. Test the Info Tips displayed in the Navigator by hovering your cursor over a symbol. The screen shot below shows how Info Tips are displayed. Set Up Default Sheet Size DxDesigner has a default sheet size for new schematic sheets. The sheet size is a property that can be changed on a case by case basis, but in the steps below you will configure the default sheet size that will be used in your projects. 1. From the Setup > Settings dialog, select Schematic Editor > New Sheets. 2. Set the Default Sheet Size to D. 3. Confirm that the Sheet Orientation is set to Landscape. 4. Enable the Automatically add border to new schematic sheets option. August 15, 2012 Page 18 of 207

19 5. Confirm that the Enable user-configurable border symbols option is enabled. The New Sheets dialog should appear as shown below. 6. Click Apply to save the settings. 7. In the Settings dialog, select Project > Borders and Zones. August 15, 2012 Page 19 of 207

20 8. Confirm that the builtin:dsheet.1 border symbol has been configured for D size sheets with a landscape orientation. The Horizontal Zones and Vertical Zones options are for DxDesigner s cross referencing via Link symbols. We will leave these alone for now. Set Up Rules for Copying DxDesigner can be configured to handle the names of copied nets in either of the following two ways: a. Net names can be copied verbatim. b. Unique net names can be automatically assigned to the copied nets. There are times when one behavior is more preferred than another, so it is helpful to be familiar with the Unique Names on Copy option. 1. Select Setup > Settings > Advanced. August 15, 2012 Page 20 of 207

21 2. Disable the Unique names on copy option. 3. Click OK to save the setting and close the Settings dialog. 4. Close the schematic and DxDesigner if you do not plan to proceed to Chapter 2. End of Chapter 1 August 15, 2012 Page 21 of 207

22 DxDesigner Tutorial for the Expedition Enterprise Flow Chapter 2: Navigating in DxDesigner The DxDesigner environment is used to optimize productivity with powerful and easy to use features. There are several ways to navigate through a design. This chapter will introduce you to several of those options. You can determine which you prefer to use. For design data completed up to this chapter, please go here: Chapter 2 Design Data. Note: You must first complete Chapter 1, and then copy this design data over the previous design data, for this design data to work properly. Exercise 1: Navigator Tree Pane As with all panes in DxDesigner, the Navigator pane is dockable. It can be undocked and moved within DxDesigner. The software will also remember heights and widths of any pane modified during a working session. This is particularly beneficial in a dual monitor configuration. The advantage of this window is the ability to view all of the design files and to jump to various pages or nets quickly and easily. 1. If DxDesigner is not running, open the DxTutorial project by double clicking the ${DxTutorial}\DxTUT_PROJ\DxTutorial.prj file. 2. If a previous project was open then select the Yes button to allow the software to close the previous documents. August 15, 2012 Page 22 of 207

23 3. Open the Navigator Tree by selecting the icon if it is not already open. 4. Double click the LMB over the name systemdesign and notice the main window displays the sheet systemdesign.1. August 15, 2012 Page 23 of 207

24 5. Next, select the icons located to the left of the systemdesign schematic, the Symbols icon, and the ARRANDALE_CPU schematic. Note: The tree should be expanded to look similar to this example. August 15, 2012 Page 24 of 207

25 6. Double click sheet 4 of the ARRANDALE_CPU schematic. The schematic pane will update to display sheet Note: The schematic sheet tabs located at the bottom display both systemdesign.1 and ARRANDALE_CPU Notice that there are 2 categories that appear in the dialog for each schematic sheet: Symbols and Nets. 9. Select the item again to expand the Symbols section of the dialog. August 15, 2012 Page 25 of 207

26 10. Select any of the symbol instances listed and notice the software automatically cross probes to that item. Note: You may need to zoom out to see the item selected during cross-probing. You can also double-click a net or symbol in the Navigator and the schematic pane will center on that net and zoom into it. Exercise 2: Zooming DxDesigner offers numerous methods for zooming in on areas of your schematic. Below you will experiment with some methods. Your mouse can be configured in a way that the zooming commands associated with the mouse wheel are consistent between both DxDesigner and Expedition PCB. The steps below will show you a few methods that you can use to zoom in and out. 1. Using the LMB click on any open area in the working area pane. 2. Press F7 and F8 on your keyboard or use the mouse wheel, if available, to zoom in or out in DxDesigner. Practice zooming in and out while using these methods. Note: As you zoom in, you may notice that the capacitors have a red box around them. The red box indicates that the symbol has been updated in the Central Library since it was added to the schematic. In Chapter 4 you will resolve the discrepancy between the schematic and the library, so disregard the red box for now. August 15, 2012 Page 26 of 207

27 DxDesigner Tutorial for the Expedition Enterprise Flow 3. Click in the schematic editor and press Home key on your keyboard (Zoom to the Full) to restore the view to the entire Schematic. Note: The keyboard hot-keys (like Home or the function keys) are sensitive only when the schematic editor pane is active. If a hot-key does not appear to work, it may be that another pane (like the Navigator) is active. All you need to do is click in the schematic editor pane and then execute the hot-key. 4. Press F9 and click and drag the LMB to define the area you wish to zoom in on. Press the Home key to return to the full view of the schematic sheet. Note: This same procedure can be done by pressing the z key, then dragging a box around the area you wish to zoom in on. Exercise 3: Help System DxDesigner offers many ways to access Help. Many dialogs have a Help button that will bring you directly to documentation concerning that dialog. The Help menu will allow you to access and search the entire documentation set for DxDesigner. SupportNet (supportnet.mentor.com) also provides access to DxDesigner documentation plus TechNotes, AppNotes, and movies on DxDesigner and all Mentor Graphics tools. 1. Notice the Help menu at the top of DxDesigner. From here you can access documentation, support, SupportNet and tips. Take a moment to view the resources available from this menu. 2. View all available shortcuts and system strokes by selecting Help > Show Bindings and Help > Show Strokes. Close the Bindings window and disable the Show Strokes mode after you have reviewed them. Note: Navigational controls can also be configured in Setup > Settings > Schematic Editor > Strokes, Pan and Zoom. Exercise 4: Window Tabs Feature One of the benefits to using DxDesigner is its ability to have several different windows displayed within the same window pane. This helps to control the flow and access of data that is available to engineers using the software. One such benefit available within DxDesigner is the ability to configure several panes in a tabbed arrangement. This allows you to enable the required dialog simply by selecting the tab representing the window pane you wish to view. August 15, 2012 Page 27 of 207

28 1. With the Navigator Tree still visible, select the icons for the DxDatabook pane, ICT Viewer pane, Properties pane, and the Output pane. This will make the respective panes visible. Your display should look like the one below. If the topology is in a different order that is okay, the following procedure will be the same. Note: You should now have 5 different panes opened up in DxDesigner along with the schematic. 2. To make things more manageable we are going to combine the DxDataBook, ICT Viewer, and Output panes into a single pane which will be located at the bottom of the window. August 15, 2012 Page 28 of 207

29 3. Using the mouse LMB, hold and select the title bar for the DxDataBook pane. 4. Drag the selected pane over the Output window. August 15, 2012 Page 29 of 207

30 Note: A placement guide will appear over each window, with additional placement guides at the edges of the application. Hovering over these boxes will place the window to the top, bottom, left, or right of the corresponding window. Placing the curser in the center of the placement guide will combine the two windows. Note: A blue tint appears on the target pane when the panes are ready to be combined. August 15, 2012 Page 30 of 207

31 5. Release the LMB to have the DxDataBook and Output panes placed alongside each other as tabs at the bottom of the Output dialog. 6. Repeat the operation with the ICT Viewer table. The results should look similar to the Output Pane shown below. 7. Disable the icons,,, and to set the Lab 2 window panes back to the way it originally was. Exercise 5: Thumbnail Viewer DxDesigner s Thumbnail pane allows you to view graphical thumbnails of schematic sheets. Thumbnails can be very useful when changing schematic sheets. 1. In the DxDesigner Navigator, double-click the systemdesign board. August 15, 2012 Page 31 of 207

32 2. In DxDesigner, select View > Thumbnails. 3. The Thumbnails pane is opened and it will display a graphical thumbnail of the systemdesign.1 schematic sheet. The Thumbnails pane will display all schematic sheets associated with the currently active hierarchical level. Since the systemdesign hierarchical level is comprised of one sheet, only one sheet is displayed in the Thumbnails pane. August 15, 2012 Page 32 of 207

33 4. In the schematic pane, right-click the ARRANDALE_CPU and choose Push. NOTE: When you push into the ARRANDALE_CPU schematic, numerous Port creation failed messages will appear in the Output pane. These occur because there are no symbols currently defined as hierarchical ports. You will resolve these issues in Chapter 5. Presently, you can ignore the messages. 5. The Thumbnails pane now displays thumbnails for each of the seven schematic sheets that comprise the ARRANDALE_CPU. August 15, 2012 Page 33 of 207

34 6. In the Thumbnails pane, double-click the ARRANDALE_CPU.7 thumbnail. This will open sheet 7 of the ARRANDALE_CPU schematic. Double-click other sheets to practice opening them with the Thumbnails pane. 7. Close the Thumbnails pane by clicking the small x in the top right corner of the Thumbnails pane. August 15, 2012 Page 34 of 207

35 Exercise 6: Find/Replace Function The Edit > Find/Replace command launches a flexible dialog that offers numerous ways to find and select objects in your schematic. 1. In DxDesigner, select Edit > Find/Replace or click the Find/Replace icon. 2. Click the More >> button to open all options. 3. Take time to familiarize yourself with the options available. August 15, 2012 Page 35 of 207

36 4. Use the Within: drop-down menu to define which part of the project you would like to search. In this case select Board: systemdesign (systemdesign). 5. In the Find what: cell type C2 and click Find All. 6. Note: The results of the search appear in the find dialog. 7. Notice that a tab on top of the design area for the sheet containing C2 has been opened. 8. In the Output window, a hyperlink appears that can be used to quickly jump to the capacitor with reference designator C2. August 15, 2012 Page 36 of 207

37 DxDesigner Tutorial for the Expedition Enterprise Flow Note: You will find capacitor C2 on the left side of the schematic sheet. 9. In the Find and Replace Text dialog change the Find what field to 22uF and click the Find All button to find all 22uF capacitors across the systemdesign Board. August 15, 2012 Page 37 of 207

38 10. Notice that all parts meeting this criterion are listed in the output window. 11. Select Window > Close All to close all of the schematic pages. Alternatively, you could click the small x to close individual sheets. August 15, 2012 Page 38 of 207

39 12. Find and Replace Text can also be used to find nets. In the dialog, activate the Use Wildcards checkbox. 13. Now enter the net name HOST*GOOD in the Find and Replace Text dialog to search across the systemdesign schematic. 14. Select the Find All button to search the entire schematic. Note: There are six instances of HOST_VTTPWRGOOD across three schematic sheets. August 15, 2012 Page 39 of 207

40 DxDesigner Tutorial for the Expedition Enterprise Flow 15. When selecting an instance of the net in the Output dialog, the associated schematic sheet is opened and that portion of the HOST_VTTPWRGOOD net is selected. This functionality allows you to check connectivity throughout your design very efficiently. 16. If you look closely at the search results, you will see that DxDesigner found pins, nets, and components named HOST_VTTPWRGOOD. In the Look in section, deselect everything but Nets and then click Find All. 17. Review the search results and you will see two hyperlinks for the two instances of net HOST_VTTPWRGOOD on two respective sheets. 18. Close the Find and Replace Text dialog. 19. Select Window > Close All to close all open schematic sheets. Exercise 7: Properties Pane and ICT Viewer The Properties Pane allows the user to change properties of one or many objects on the schematic. The ICT Viewer can be used to find elements within your design. These two panes can be used together to select and edit or add properties on multiple parts in your schematic. 1. In the Navigator, double-click the systemdesign board. 2. Select the Properties icon or type CTRL-ALT-A as a hotkey executed from the keyboard. 3. Select the ICT Viewer icon. August 15, 2012 Page 40 of 207

41 DxDesigner Tutorial for the Expedition Enterprise Flow 4. For this exercise you can close all panes except the Navigator, the schematic editor, ICT Viewer and Properties panes. Note: The scope of the ICT Viewer is controlled by the Navigator. So make sure that you have selected the systemdesign schematic in the Navigator. Otherwise, you will not be viewing all of the parts in the design. 5. In the ICT Viewer pane, select the Symbol Properties tab on the bottom of the window. August 15, 2012 Page 41 of 207

42 6. Select all the resistors with a value of 10K by scrolling to find the Value column in the ICT Viewer. Click the small arrow in the first row. This will open a list of available values. You can either select 10K from the list or you can type it into the free text field. August 15, 2012 Page 42 of 207

43 7. A filter has been applied and now only the 10K resistors are shown. Note: You can resize the width of any of the columns in the ICT Viewer by positioning the mouse cursor over the boundary between columns and click and dragging the left or right when you see the cursor icon appear as a double-ended arrow. 8. In the ICT Viewer, select one of the resistors with a Part Number of by selecting the resistor s ID ($xxxx) from the leftmost column. August 15, 2012 Page 43 of 207

44 9. The property values for that part are shown in the Properties window. 10. Values can be changed by clicking the cell in the Properties window and typing a new value. Change the resistor s Rating property from 125mW to 250mW in the Value column of the Properties window. 11. After entering the new value click into another cell to apply the change. 12. Select Edit > Undo or press the u key on your keyboard to restore the original value of 125mW to the resistor. August 15, 2012 Page 44 of 207

45 13. Select all 10K resistors by clicking the top row in the ICT Viewer and then holding the Shift key and clicking the bottom row in the ICT Viewer. You may need to use the scroll bar to view the bottom of the list of resistors in the ICT Viewer. Remember that the ICT Viewer s scope is controlled by the Navigator. If you don t see 23 resistors in the list, you should check the Navigator and make sure that systemdesign is selected. August 15, 2012 Page 45 of 207

46 14. After doing this, all resistor properties can be modified simultaneously by editing the desired property from within the Properties dialog. To practice this, select the Tolerance property row in the Properties dialog. 15. Change the value to 1% and click Enter on your keyboard. August 15, 2012 Page 46 of 207

47 16. In the Properties dialog enable the visibility of the Package_Type value by clicking the checkbox in the Value cell such that a check mark is in the checkbox. 17. Inspect one of the resistors in the schematic to confirm that the Package_Type value is now visible. 18. In the ICT Viewer select all of the 10K resistors and disable the visibility of the Package_Type value. 19. In the Navigator, select systemdesign. August 15, 2012 Page 47 of 207

48 20. In the schematic pane, right-click on the ARRANDALE_CPU and choose Push. Note: When you push into the ARRANDALE_CPU schematic, numerous Port creation failed messages will appear in the Output pane. These occur because there are no symbols currently defined as hierarchical ports. You will resolve these issues in Chapter 5. Presently, you can ignore the messages. 21. Press the PageDn key on the keyboard until you get to Sheet 3 of the ARRANDALE_CPU schematic. The active sheet name will show at the bottom edge of DxDesigner. August 15, 2012 Page 48 of 207

49 22. Using the LMB, click on either of the two large symbols. 23. Note: The ARRANDALE_CPU part is a very large part which makes it impractical to capture as a single symbol. Therefore, the librarian has fractured this part into multiple symbols. Two of those symbols appear on sheet 3 of the ARRANDALE_CPU schematic. Note: Once a symbol is selected, its properties will appear in the Properties editor. August 15, 2012 Page 49 of 207

50 24. The Properties window will update with selections in the schematic or the ICT Viewer. 25. Close the Properties window by selecting the in the upper right hand corner of this pane. 26. Close the ICT Viewer. August 15, 2012 Page 50 of 207

51 27. Select Window > Close All to close all open schematics. Note: At no time have you had to save your work in DxDesigner. DxDesigner is constantly saving your data. As you complete an action like moving a part DxDesigner immediately writes that change into the schematic database. End of Chapter 2 August 15, 2012 Page 51 of 207

52 DxDesigner Tutorial for the Expedition Enterprise Flow Chapter 3: DxDesigner - Selecting and Verifying Parts with DxDataBook DxDataBook is a component information system that allows companies to benefit from a centralized component database system. The DxDataBook utility allows customers to manage their library data more efficiently than ever before. It increases efficiency by decreasing the number of symbols required to support the parts in their design environment. DxDataBook connects to any ODBC compliant database and makes the necessary content available to aid in the part selection process. When the part is added to the schematic, the property data is also added so the part is complete when it is released onto the schematic. DxDataBook also provides component verification checks which ensure the property data attached to the symbol in the schematic matches the respective property values in the Centralized ODBC compliant database. This prevents incomplete or inaccurate data from being passed into the PCB design phase. For design data completed up to this chapter, please go here: Chapter 3 Design Data. Note: You must first complete Chapter 1, and then copy this design data over the previous design data, for this design data to work properly. Exercise 1: Configure DxDataBook The system allows for easy searching and selecting of components. It can tie into a company s purchasing database so that engineering can make more intelligent part selections based on lead time, cost, stock availability, etc. 1. If DxDesigner is not running, open the DxTutorial project by double clicking the ${DxTutorial}\DxTUT_PROJ\DxTutorial.prj file. August 15, 2012 Page 52 of 207

53 2. Activate the Navigator icon and the DxDataBook icon. 3. In the Navigator, double-click the systemdesign board to open the systemdesign.1 schematic. 4. If the Output pane is open select the Output pane icon to close it. 5. Make sure that DxDataBook is connected to the SampleLib.dbc configuration file. You can verify this by looking at the bottom left corner of DxDataBook. August 15, 2012 Page 53 of 207

54 6. If SampleLib.dbc is not listed in DxDataBook, then select Setup > Settings > Project > DxDataBook and set the DxDataBook configuration to ${DxTUTORIAL}\DxTUT_Lib\SampleLib.dbc. DxDataBook relies on some settings stored in your Windows Registry. In the steps below we ll inspect the settings of your Windows Registry to ensure that DxDataBook will display and annotate component properties in a way that is consistent with the instructions in this tutorial. 7. In the DxDataBook pane, right-click and choose Properties. August 15, 2012 Page 54 of 207

55 8. In the DxDataBook Properties dialog, click the Appearance tab. 9. Confirm that the Display option is set as DxDesigner Property Names. Set that option if it is not already configured on your machine. 10. Enable the Display numeric values with magnitude and the Enable DxDataBook Window Column Tooltip options. Click OK to close the DxDataBook Properties dialog. August 15, 2012 Page 55 of 207

56 DxDesigner Tutorial for the Expedition Enterprise Flow Exercise 2: DxDataBook Libraries The Library drop-down menu contains a list of all available libraries as described in the database source. These libraries are defined as Tables directly in the Microsoft Access database that is used for this tutorial. The list and organization of the libraries is configured by the DxDesigner librarian or tools administrator. 1. Choose Digital_Logic from the Library drop-down menu. Note: The system now searches the database and lists all the components in this library. Note: Matches in the lower right side of the DxDataBook grid indicates how many parts meet the current filter criteria. August 15, 2012 Page 56 of 207

57 Exercise 3: Component Selection with DxDataBook When using a standard library configuration without DxDataBook, you must take the time to enter properties for each instance of a part. This can be both time consuming and error prone. This process also requires the creation of numerous extra schematic symbols. In this exercise you will see how DxDataBook reduces the need for extra symbols by having generic symbols populated with property values from a database. You will also see how easy it is to search for and select specific parts from a large list. 1. From the Library drop-down menu select the Resistor library. 2. Select the Query Builder button to start setting the query criteria. 3. With the Query Builder dialog open, click the Condition button. August 15, 2012 Page 57 of 207

58 4. Select the drop-down arrows in each setting in the dialog so it matches the example below (Package_Type; =; 0402). Select the Add button to set the criterion. Note: This will place the search criterion into the dialog as shown, so it can be applied. 5. Select the OK button to activate the search based on the criterion. Note: The resulting data is based on Packge_Type equaling August 15, 2012 Page 58 of 207

59 6. Now narrow the search to find resistors with Value=10K and Package_Type=0402. Launch the Query Builder again and click the AND button. 7. Click the Condition button to enable the drop-down menus in the Query Builder. 8. Select the drop-down arrows in each setting in the dialog so it matches the example below (Value =; 10K). 9. Select the Add button to set the criterion. August 15, 2012 Page 59 of 207

60 DxDesigner Tutorial for the Expedition Enterprise Flow 10. Select the OK button to apply the additional search based on the new criterion. Note: The list of available parts has been reduced to a single part. 11. Using the LMB select the Part Notice the entire line is highlighted and the symbol appears in the symbol preview on the right of the DxDataBook pane. 12. Using the LMB, click and drag the symbol in the preview window and place it on the schematic. August 15, 2012 Page 60 of 207

61 13. Click on the Properties icon or use the modeless command CTRL-ALT-A to open the Properties window. All the properties are on the symbol. These properties were added to the generic symbol by the Microsoft Access database when the part was added to the schematic. The user does not have to worry about making manual errors in adding the properties. Note: When symbols are added to a schematic, DxDesigner assigns a unique Id to them. If you compare your schematic to the screenshots below, it is unlikely that the Id properties will match. This is not a problem so you can disregard any discrepancies between your Id properties and the Id properties shown in the screenshots below. August 15, 2012 Page 61 of 207

62 14. While in the Properties editor, change the Value property field from 10K to 107K by entering the new value in the Value column. Note: You made a unique change to a part so the part number no longer matches the resistor s value. This condition could lead to a very expensive problem due to the way parts are ordered through a company s purchasing department. Part numbers that do not match corresponding properties generally lead to overstocks and delays in schedule. Both are costly and can be avoided if a DxDataBook configuration is in place. Over the following steps you will look at how DxDataBook can find these inconsistencies and allow you to resolve them quickly. 15. Drag another resistor from DxDataBook (Part Number = ) onto the schematic sheet so there are two new ones displayed. 16. Change the Libraries: setting from Resistors to Capacitor. 17. August 15, 2012 Page 62 of 207

63 18. Now assume you need a decoupling capacitor, but have not decided on what value of decoupling capacitor to use. In DxDataBook, select the drop-down menu under the Catalog_Group column and select CAP_FIXED and press Enter on your keyboard to execute the query. 19. In DxDataBook, use the Dx_Symbol drop-down menu to select passive_discrete:capacitor 20. In DxDataBook, use the drop-down menu below the symbol preview to select the capacitor.2 symbol. August 15, 2012 Page 63 of 207

64 DxDesigner Tutorial for the Expedition Enterprise Flow Note: The librarian has created symbols for both vertical and horizontal orientation. It is good practice to select the properly oriented symbol when you add a part. Doing so will save you the effort of rotating parts manually. Additionally, the text on your symbols will be oriented to make it easy to read the schematic. 21. Select any capacitor listed in DxDataBook and click on the Add new component with common Properties icon to add a generic component to the schematic. With the new part active on your cursor, move both the cursor and the symbol over the working area and select the LMB to complete the part placement. 22. Right-click after the capacitor has been added to the schematic to return the cursor to the Select mode. August 15, 2012 Page 64 of 207

65 23. Select the capacitor and look at the Properties editor. You will notice the capacitor is missing Value and several other properties. DxDataBook can run a complete verification to ensure all parts are compliant with the database. 24. DxDataBook has the ability to run verification on a group of selected items, a single page, or an entire design. For this exercise you will do a verification of the parts we just placed. 25. Select the Filter icon located on the toolbar. Enable only the Symbol check box. August 15, 2012 Page 65 of 207

66 DxDesigner Tutorial for the Expedition Enterprise Flow 26. Do not close the Selection Filter dialog. It will help to remind you that you need to restore the ability to select the other object types. 27. While using the LMB drag a select box around the three symbols we just added via DxDataBook. 28. Restore the Selection Filter to the default settings by enabling the All checkbox and disabling the Pin checkbox. The selection filter should appear as shown below. 29. Close the Selection Filter by clicking the x in the upper right corner of the dialog. August 15, 2012 Page 66 of 207

67 30. Click on the New Live Verification Window icon located in the DxDataBook dialog. Note: This button is also used for verifying an entire page if no items are selected when it is activated. 31. A new window will open showing the three parts color-coded. If we click on any of the parts, that part is highlighted in the schematic. Indicates a component has multiple matches. This is the generic component we added. Indicates the properties on the schematic match the database and only one part matches. Indicates that there is a conflict between the database and the schematic and no parts match. This is the part where we changed the Value so it no longer matches the Part Number. 32. First, you will fix the problem with the capacitor which is not correctly specified. Using the LMB, double-click on the Yellow Circle. 33. On the right hand side a search window opens up with the common properties automatically applied as filters. August 15, 2012 Page 67 of 207

68 34. Using the LMB, select any part listed in the DxDataBook dialog. 35. Using the LMB select the Annotate Component with all Properties to add the missing part information. Notice the circle changes from yellow to green and the Properties Editor now shows the capacitor as a completely defined component. 36. Double-click the row that has the red circle. DxDataBook has detected that the resistor s value of 107K does not exist in DxDataBook s database. August 15, 2012 Page 68 of 207

69 37. In the right side of DxDataBook s Verify tab, scroll to the right and notice that the verify routine has found a conflict. The Value is colored red because it does not match the database. Note: You may have to adjust the column widths to make read the property values on the part. 38. Using the LMB, scroll to the Value property name, click the RMB and select Remove Condition. August 15, 2012 Page 69 of 207

70 39. The system will search the database and find the part that matches the previously defined conditions. Note: The verification routine has found a single part. 40. Using the LMB, click on the part number. 41. Using the LMB, select the Annotate component with All Properties icon to change to the new part. 42. We have now corrected the problem of the mismatched properties on the resistor. In Live Verification mode, DxDataBook automatically re-verifies the parts and will show that all three parts match the database. 43. Select all three parts you placed using the CTRL + LMB keys. 44. Press the Delete key to delete the three parts you added during this exercise. 45. If you are going to continue on to Chapter 4, you can leave the systemdesign schematic open. Otherwise, close DxDesigner. End of Chapter 3 August 15, 2012 Page 70 of 207

71 DxDesigner Tutorial for the Expedition Enterprise Flow Chapter 4: DxDesigner Schematic Manipulation DxDesigner is a comprehensive schematic entry tool which combines a feature rich environment with an easy to use GUI. DxDesigner is simple to navigate whether you are adding parts, connections, busses or text. For design data completed up to this chapter, please go here: Chapter 4 Design Data. Note: You must first complete Chapter 1, and then copy this design data over the previous design data, for this design data to work properly. Exercise 1: Creating a New Schematic Note: The schematic shown below will be constructed during the following exercises. 1. If DxDesigner is not running, open the DxTutorial project by double clicking the ${DxTutorial}\DxTUT_PROJ\DxTutorial.prj file. August 15, 2012 Page 71 of 207

72 DxDesigner Tutorial for the Expedition Enterprise Flow 2. In DxDesigner, click the New icon, or click the down arrow and then Schematic. 3. The schematic will initially be named Schematic1. Right click on the Schematic and select Rename. Type d2a_converter over the Schematic1 name. Note: The d2a_converter is now a schematic in the DxTutorial project, but it is not yet integrated into the systemdesign board. In this lab you will create the d2a_converter schematic and in Chapter 5 you will integrate this schematic into the systemdesign board design. August 15, 2012 Page 72 of 207

73 DxDesigner Tutorial for the Expedition Enterprise Flow Exercise 2: Adding a Sheet Border Adding borders into a schematic can be done several ways. The process can be automatic or manual. You can change borders at any time to reflect a sheet size modification. In the following steps you will change the size of this new sheet to a C sized sheet. 1. Activate the Properties dialog for the schematic sheet by double-clicking the LMB in any blank area of the schematic. 2. Change the Drawing Size to C by selecting the drop-down in the Properties window. 3. RMB and pick Insert Border from the pop-up menu. The pre-defined C sheet border will replace the D sheet border. Note: When adding a border using this method, DxDesigner will insert the symbol for the current sheet size as defined in Setup > Settings > Project > Borders and Zones. This menu also stores the definitions for automatic border insertion whose mapping(s) should be embedded in your company s template project. August 15, 2012 Page 73 of 207

74 DxDesigner Tutorial for the Expedition Enterprise Flow 4. If needed, press F8 a few times to Zoom Out or hit the Home button to change the view so it centers on the format. Exercise 3: Adding Components 1. If DxDataBook is not open, invoke the DxDataBook dialog by clicking the icon. 2. In the Search tab of DxDataBook, select the Capacitor library. August 15, 2012 Page 74 of 207

75 DxDesigner Tutorial for the Expedition Enterprise Flow 3. In the Value column of DxDataBook, type the value of 6.8pF and press Enter. Note: The library contains a single 6.8pF capacitor. 4. In DxDataBook, select the row corresponding to the 6.8pF capacitor. 5. Drag and drop the 6.8pF capacitor from the DxDataBook symbol preview pane onto the schematic. August 15, 2012 Page 75 of 207

76 6. Zoom in on the capacitor by entering a capital Z on the keyboard. The hot-key Z is a helpful command that will zoom in on whatever objects are selected in the schematic pane. Make sure that you are aware of the state of Caps Lock because some commands are case-sensitive. Note: There is red box outlining the capacitor. This is how DxDesigner alerts you that symbols have been changed in the library. If you saw this in one of your designs it would be wise to contact your librarian to find out how the symbol was changed. In this case, default values for some symbol properties have been added to the symbol. This has no impact on the integrity of the schematic, but DxDesigner will flag any change to a symbol file with a red box. In the following steps you will execute a command that will accept the symbol changes and clear the red box. August 15, 2012 Page 76 of 207

77 7. Select Tools > Update Symbols. The Update Symbols command will inspect your project and identify all symbols that have been updated in the Central Library since the time they were placed in the schematic. The Component definition update dialog allows you to select which symbols you would like to update. 8. With the capacitor.1 checkbox selected, click OK in the Component definition update dialog to update the symbol. When the update process concludes, the red box will disappear. 9. In DxDataBook, right-click and choose Remove All Conditions to clear the current query. 10. In DxDataBook, search the Capacitor library for a capacitor with a Value of 100nF and a Tolerance of 20%. Add it to the schematic. 11. Switch the DxDataBook library to the AD_DA library. Here you will find only one part, the da_8bit.1 symbol. August 15, 2012 Page 77 of 207

78 DxDesigner Tutorial for the Expedition Enterprise Flow 12. Before you add the da_8bit.1 symbol to the schematic, select the pin numbers for the part from the Slot drop-down menu. Note: If you add a part from DxDataBook without selecting a slot, it will have no pin numbers. This is not necessarily a problem because the Packager will add any pin numbers that are missing prior to opening the design in Expedition PCB. However, most schematic designers want to have the pin numbers on their parts when they are added to the schematic, so it is good practice to select the Slot option when you are adding symbols to your schematic. 13. Drag and drop the da_8bit.1 symbol onto the schematic. 14. Arrange the three components as shown in the screenshot below. 15. Close the DxDataBook dialog. August 15, 2012 Page 78 of 207

79 DxDesigner Tutorial for the Expedition Enterprise Flow Exercise 4: Adding Power and Ground Connections. 1. Open the Settings dialog using Setup > Settings. 2. Navigate to Project > Special Components. Then, select Power from the dropdown menu and click the New icon. 3. The Power Symbol dialog will open and allow you to browse the libraries for a power symbol. Select the pwr.1 symbol from the builtin library. Click OK. 4. Follow the same process but this time select Ground in the Special Components dialog. Then, from the builtin library select gnd.1 and select OK. August 15, 2012 Page 79 of 207

80 5. Select the OK button to exit the Settings dialog. Note: Now, in your toolbar for DxDesigner the Special Components icon display the pwr.1 and gnd.1 symbols. 6. Click on the Special Components icon and select the builtin:pwr.1. will 7. A power pin will be attached to your cursor. Select the LMB to place the power symbol in the working area. When you have placed it click RMB to exit the power pin mode. Note: When you add a pin using this method, DxDesigner enters a mode where a pin is added each time you click the LMB. You can exit that mode by clicking the RMB or by pressing the Esc key. 8. Follow the same steps to add a Ground symbol to the schematic. August 15, 2012 Page 80 of 207

81 DxDesigner Tutorial for the Expedition Enterprise Flow Exercise 5: Moving Components To move components: A. Click and hold the LMB down while the cursor is over the part you wish to move. Drag the cursor to the desired location. B. Release the LMB to drop the part. 1. Arrange the components as seen in the figure below. Note: You can select multiple components simultaneously by holding down the CTRL key while selecting all desired parts with the LMB. When you have selected all of the intended parts release both the CTRL key and the LMB. Click any of the selected parts with the LMB and drag the parts to a new location. Release the LMB to place the parts. 2. Use the method described above to move all of the parts to the center of the sheet. 3. When you have moved the components, click in vacant area of the schematic to deselect all of the components. August 15, 2012 Page 81 of 207

82 DxDesigner Tutorial for the Expedition Enterprise Flow Exercise 6: Connecting the Components with Nets There are a few ways to add nets to components. This section will experiment with a few different options. Connecting by Abutment 1. Click the Zoom Area icon and draw a frame around the symbols you added. This will cause DxDesigner to zoom in around those parts. 2. Select the power pin (pwr.1). 3. Select and hold the LMB and drag the first power pin to the point where the power pin touches the end of pin 13 on the da_8bit.1 symbol. A purple star will appear letting you know that a connection is going to be made when the power pin is placed at that location. Note: It is important that the ends of the two pins share the same grid location. If the pins overlap each other, they will not be joined. 4. Place the power pin by releasing the LMB. August 15, 2012 Page 82 of 207

83 5. Select the power pin again and drag it away from the IC. The pins are automatically connected as we drag the power pin away from the IC symbol. Release the LMB to place the power pin approximately 10 grid points above the IC. Note: If your connection does not look like the screenshot above, repeat steps 3 through 5 above. 6. Use the Abutment method to connect the ground pin to pin 6 of the IC component. Creating Nets Using the Right Mouse Button DxDesigner can create nets if you right-click the mouse while the cursor is near the end of a pin or a dangling net. 1. Position the mouse cursor above pin 16 of the IC, but make sure that the cursor is not touching or on top of the pin. August 15, 2012 Page 83 of 207

84 DxDesigner Tutorial for the Expedition Enterprise Flow 2. Click the RMB and move the cursor. A net will be connected between the mouse cursor and pin 16. Note: If the Strokes feature is enabled, you may end up issuing a stroke command instead of drawing a net. The key to ensuring that you draw a net (rather than issue a stroke command) is to make sure that: a. The mouse cursor is not on the pin, but near the end of the pin. b. The mouse cursor is stationary when you click the RMB. 3. Move the mouse cursor upward three or four grid points. The net will follow the mouse without your having to hold a mouse button. 4. Click the RMB and move the cursor to the left. This will allow you to create a bend in the net. Note: You could have simply moved the cursor to the left and the net would turn to the left. Clicking the RMB to turn the net has the advantage of precisely determining where the net bend occurs. 5. Position the cursor on the net between pin 13 and the power pin and click the LMB to complete the connection. The net should appear as shown below. August 15, 2012 Page 84 of 207

85 6. Use the same method to connect the ground pin to pins 6 and 2 of the IC. Creating Nets using Net Mode 1. Select the Net icon (or type n using the keyboard) to put the software in Add Net mode. This mode suspends all other LMB functions in the schematic editor window. Below you will use the Add Net mode to add a net to pin 14 on the IC. 2. Position the cursor at pin Click and hold the LMB and move the mouse cursor to the right. This will create a net. 4. Release the LMB to terminate the net. August 15, 2012 Page 85 of 207

86 5. Follow the process outlined in steps outlined above to add straight nets to pins 1, 5, and 15 on the IC. 6. Click the RMB to exit the net mode. Alternatively, you can press the ESC key on the keyboard or select the Select icon to exit net mode. Exercise 7: Naming Nets 1. Double-click the net connected to pin 14 of the IC. This will open the Properties dialog and display the properties associated with the net. August 15, 2012 Page 86 of 207

87 2. Enter A as the value for the Name property. 3. In the schematic editor, select only the name (A) and move it away from the net and release LMB. Notice that a dashed line indicates the net to which the Name belongs. 1. Move the net name back to its original position on top of the net. 2. Select the net and move it. Note that the net name moves along with the net. 3. Return the net to its original position. You can do this either manually or by selecting Edit > Undo or by pressing CTRL + Z. 4. In the Properties dialog click the checkbox next to the Name value. This will disable the visibility of the Name. August 15, 2012 Page 87 of 207

88 5. With net A selected, note that the lower left corner of the schematic window reports the name and ID of the net. Note: The Id of your net may differ from that shown in the screenshot above. 6. Select the net connected to pin 15 and name it A. August 15, 2012 Page 88 of 207

89 7. In the Properties dialog, change the Name Inverted property to True by clicking the LMB in the Value cell of the Name Inverted property. Note that this changes the Name property to ~A and the name in the schematic editor is displayed with an inversion bar. 8. In the Properties dialog disable the visibility for this net name. August 15, 2012 Page 89 of 207

90 Adding Names using the Navigator 1. Click the net that is attached to pin 5 of the IC. 2. Notice that the net ID will be highlighted in the Navigator. Note: Remember that the net IDs in your schematic may differ from those shown in the screenshots. Such differences are not a problem. 3. In the Navigator, position the cursor over the net s ID in the Navigator and use the RMB menu to select Rename. Rename the net CLK and click Enter. DxDesigner will display the text case that you use. Use uppercase letters for your net names in this tutorial. 4. Select the net in the schematic pane and use the Properties dialog to disable the visibility of CLK. 5. Use the method described above in steps 1 through 3 to add the name V_REF to the net connected to pin 1 of the IC. 6. Disable the visibility of V_REF. August 15, 2012 Page 90 of 207

91 Exercise 8: Modifying Properties Property Visibility 1. If not already open, activate the Properties editor by selecting the Properties icon or by entering the modeless command CTRL-ALT-A. 2. Using the LMB, select the IC. Note: The Properties for that component are displayed in the Property editor 3. To make a property type visible you can check the box next to the desired property. Check the box next to Package_Type. Notice Package_Type is now shown below the symbol. August 15, 2012 Page 91 of 207

92 4. Make only the value visible by checking the box next to 16SO4 and unchecking the box next to Package_Type. Modifying Property Values 1. Select the Power pin symbol. 2. In the Properties dialog, set the Global Signal Name property to 5V. 3. Make sure that the Global Signal Name value is visible. Note: The Global Signal Name property will propagate its value to be the name of any net that connects to this pin. The ground pin symbol also has a Global Signal Name property; however, it will not be edited here because it has the desired value, GND, already. August 15, 2012 Page 92 of 207

93 DxDesigner Tutorial for the Expedition Enterprise Flow Adding New Properties 1. Multiple select the IC and the two capacitors by first selecting one component and then CTRL+LMB on each of the other two components. 2. The Properties dialog displays the properties for the three components. If any of the properties among the selected objects have differing values the property value is listed as <Multiple Values>. 3. In the Properties dialog, select the bottommost cell in the Property column. 4. A menu will appear with a list of properties that can be added to these components. Select Cluster from the list. This will add the Cluster property to each of the components. August 15, 2012 Page 93 of 207

94 5. While all three components are still selected, set the Value of Cluster to DA_Converter. Exercise 9: Working with Busses 1. Invoke the Bus mode by clicking the Bus icon. 2. Draw a vertical bus to the left of the IC symbol. 3. Continue the bus by adding a horizontal segment at the top of the vertical segment. Tip: Be sure to extend the vertical bus segment so that it is aligned with pin 7 down to pin 12 of the IC. August 15, 2012 Page 94 of 207

95 DxDesigner Tutorial for the Expedition Enterprise Flow 4. Exit the Bus mode by pressing Esc on the keyboard. 5. Select the horizontal segment of the bus. 6. In the Properties dialog, name the bus A_CHANNEL[7:0]. This creates a bus comprised of net names: A_CHANNEL7, A_CHANNEL6, A_CHANNEL0. 7. Select the bus name in the schematic. This will cause the bus segment to become deselected and the Properties dialog will display the properties associated with the bus name (rather than the bus object). 8. Set the Size property to DxDesigner will fill in the units automatically. 9. Reposition the bus name so it sits above the horizontal bus segment. August 15, 2012 Page 95 of 207

96 10. Use the RMB to click the vertical bus segment and choose Rip Nets from the popup menu. 11. Click OK in the Rip Nets dialog and move the resultant nets so they connect to the pins on the left side of the IC. 12. Click the LMB to complete the connection to the IC pins. 13. If the Net names are too close to the IC or overlap with the IC, select the vertical bus segment and move it to the left. The net names will follow the bus segment. August 15, 2012 Page 96 of 207

97 DxDesigner Tutorial for the Expedition Enterprise Flow Exercise 10: Copying Symbols DxDesigner offers many ways to copy objects. Below we will practice with two methods: Copy and Paste and Duplication. The Copy (CTRL+C) and Paste (CTRL+V) commands work with the operating system s paste buffer. These commands are particularly helpful when you intend to copy and paste between different schematic sheets or different schematic projects. The Duplication method (CTRL+LMB and Drag) is efficient if you intend to copy objects within a schematic sheet. 1. Hold the CTRL key down and select the power and ground pin symbols. This causes the two symbols to be selected as a group. 2. Press CTRL+C on the keyboard. Alternatively, you could position your cursor over one of the selected symbols and click the RMB and choose Copy. 3. Press CTRL+V on the keyboard or click the RMB and choose Paste. Note: Nothing happens! Unlike a text editor, DxDesigner does not have an active insertion point. Therefore, you need to click the LMB to complete the Paste command. 4. Click and hold the LMB and move your cursor toward the capacitor symbols. 5. Release the LMB to place the copied power and ground pins. 6. Position the power and ground pins as shown in the screenshot below. August 15, 2012 Page 97 of 207

98 7. Use your choice of net drawing commands to make the connections shown below. Review the steps in Exercise 6 of this chapter if needed. 8. Zoom out to see the entire schematic. You can do this by clicking the Fit All icon, or by pressing the Home button on your keyboard. The schematic should appear as shown below. August 15, 2012 Page 98 of 207

99 DxDesigner Tutorial for the Expedition Enterprise Flow Now, assume it has been decided that the design will have two channels. Therefore, you will copy this circuit and rename the nets and bus to account for the second channel. 9. To give you more room on this page, change the sheet size back to a D sheet. Double-click a blank area of the schematic to view the schematic properties in the Properties dialog. 10. Change the Drawing Size to D. Notice that the C size sheet border remains. 11. Click the RMB and choose Insert Border. As seen earlier, this will replace the current border with the pre-defined border for the now D size sheet. 12. Select the entire circuitry and then click and drag the circuitry upward to make room for the second channel circuit. 13. With all circuitry still selected, press and hold the CTRL key then position the cursor on the IC and press and hold the LMB (while you are still holding the CTRL key). 14. Move the mouse cursor downward and a duplicate copy will appear attached to your cursor. Position the new circuit below the original circuit. August 15, 2012 Page 99 of 207

100 Exercise 11: Renaming Properties Recall in Chapter 1 that we disabled the Unique names on copy. Since we disabled that mode, at this point there are two copies of the Channel A circuit, including duplicate net names. In the steps below you will rename the net names to make a new channel that will be called Channel B. 1. Select the horizontal bus segment of the lower circuit. 2. In the Properties dialog, rename the bus B_CHANNEL[7:0]. Notice that the net names that attach to the bus are automatically changed. 3. Use the same method to change the names of A and ~A to B and ~B, respectively. The remaining net names do not need to be changed. 4. Disable the visibility of net names B and ~B. August 15, 2012 Page 100 of 207

101 Exercise 12: Completing the Channel Circuits 1. Use the net drawing techniques you have learned to make the final connections shown below. This involves joining the V_REF and CLK nets. Move nets and net names as needed to give the schematic an orderly appearance. August 15, 2012 Page 101 of 207

102 Exercise 13: Using Arrays The Array feature can be used to add components and to add net labels. It can also be used to add multiple objects. To practice using DxDesigner s Array feature, you will create an array of capacitors on a different sheet of the systemdesign schematic. The circuit that you will create is shown below. 1. Open the ddr2_interface schematic by double-clicking its yellow icon in the Blocks tree of the DxDesigner Navigator. August 15, 2012 Page 102 of 207

103 DxDesigner Tutorial for the Expedition Enterprise Flow 2. Open DxDataBook by clicking its icon. 3. In the Search tab of DxDataBook, select the Capacitor library. 4. Type 10nF in the Value column and press Enter to execute the query. A single capacitor appears in the list below. 5. Select the row associated with part number Click the N icon to the left of the symbol preview pane. The N icon will cause net stubs to appear on each pin of any part added from DxDataBook. If you subsequently click the L icon, net names will automatically appear on the net stubs. In this case, you only need to have the net stubs, not the names, so you will not use the L icon at this time. 7. Click and drag the capacitor from the preview pane onto the schematic. Note that net stubs are added to the capacitor. August 15, 2012 Page 103 of 207

104 DxDesigner Tutorial for the Expedition Enterprise Flow 8. Position the capacitor toward the top right portion of the schematic sheet. 9. Add horizontal net segments to the top and bottom net segments attached to the capacitor. Make sure that the two segments are of equal length. 10. Select the capacitor and all of the net segments that are attached to it. 11. Select the Array button to begin the arraying process. 12. Fill in the dialog as seen below: Rows = 4, Columns = 4. Click OK. August 15, 2012 Page 104 of 207

105 13. Sixteen capacitors arranged in a 4 by 4 array are attached to your cursor. Move your mouse cursor such that there is no gap between columns and there is a reasonable gap between rows (0.1 in. to 0.3 in.). 14. When you have the capacitors in the desired position, click the LMB to place them. August 15, 2012 Page 105 of 207

106 15. Delete the capacitor on the bottom right of the array and delete the lower net stub on each of the rows. 16. Add a power pin symbol and a ground pin symbol to the schematic. 17. Double-click the power pin symbol and set the Global Signal Name to 3V3. August 15, 2012 Page 106 of 207

107 18. Add the net segments shown below to connect the power and ground pins to the capacitors. 19. Select Window > Close All. 20. Close DxDesigner unless you intend to continue on to Chapter 5. Note: Remember, at no time have you had to save your work in DxDesigner. DxDesigner is constantly saving each time you complete a task. End of Chapter 4 August 15, 2012 Page 107 of 207

108 DxDesigner Tutorial for the Expedition Enterprise Flow Chapter 5: DxDesigner Hierarchical Design A hierarchical design methodology can greatly enhance a design flow by both partitioning a design in a logical way and by taking advantage of schematic reuse. Hierarchical schematics are also better suited for collaborative or team design approaches. DxDesigner has numerous features that both support and simplify hierarchical design methodologies. In this chapter you will learn some of these features and methods. For design data completed up to this chapter, please go here: Chapter 5 Design Data. Note: You must first complete Chapter 1, and then copy this design data over the previous design data, for this design data to work properly. Exercise 1: Preparing for Hierarchical Design Hierarchical ports are required in schematics to identify which nets will drive or be driven by nets from a higher level schematic. Therefore, whether using bottom-up or top-down hierarchical design methods, port symbols must be available to schematic designers so that they can add them to the appropriate nets and busses. In this exercise you will configure your project to use input, output, and bi-directional hierarchical ports. Normally, the pointers to hierarchical port symbols should be preconfigured by your tools administrator or librarian and stored in the speccomps.ini file. However, for the purpose of this exercise, you will manually define these settings for your project. 1. If DxDesigner is not running, open the DxTutorial project by double clicking the ${DxTutorial}\DxTUT_PROJ\DxTutorial.prj file. 2. In the DxDesigner Navigator, double-click the d2a_converter block that you created in Chapter Select Setup > Settings > Project > Special Components. August 15, 2012 Page 108 of 207

109 4. With Port IN as the component type, click the New (Insert) icon. 5. In the Port IN dialog, unfold the builtin library and select the hier_in.1 symbol. 6. Click Apply to add the hier_in.1 port symbol to the Special Components list. 7. Change the port type to Port OUT and follow the same process to add hier_out.1 to the Port OUT category. 8. Change the port type to Port BI and follow the same process to add hier_bi.1 to the Port BI category. Click OK to exit the Settings dialog. August 15, 2012 Page 109 of 207

110 9. This completes the port definitions that you will need for this tutorial. Click on the Special Components icon to confirm that the three hierarchical pins are now available in the menu. Exercise 2: Bottom-Up Hierarchical Design Bottom-up hierarchical design involves first creating a schematic and then creating a hierarchical symbol that represents that schematic. Bottom-up design tends to be a good method for users who are new to hierarchical design since it starts with the familiar task of creating a schematic. In this exercise you will return to the d2a_converter schematic to build it into a hierarchical structure. Simply put, the process of creating a bottom-up hierarchy involves the following steps: a. Create a schematic b. Add port symbols to nets/ busses that traverse to the higher level c. Generate the hierarchical symbol In Chapter 4 you created the d2a_converter schematic, so in this exercise you will continue the effort by adding hierarchical ports to the schematic s nets and busses. August 15, 2012 Page 110 of 207

111 1. In the d2a_converter schematic, multiple select the CLK, A_CHANNEL[7:0], and B_CHANNEL[7:0] bus/net segments shown below. Note: Remember that you can select multiple objects by holding down the CTRL key and selecting two or more objects. August 15, 2012 Page 111 of 207

112 2. Click the Special Components icon and select the IN: builtin:hier_in.1 symbol from the list. Note: The net and bus names are added to the hierarchical port. 3. Select the output nets A, ~A, B, and ~B. 4. Use the Special Components icon and select the IN: builtin:hier_out.1 symbol from the list. 5. Select the V_REF net. August 15, 2012 Page 112 of 207

113 6. Use the Special Components icon and select the BI: builtin:hier_bi.1 symbol from the list. 7. Position the names on the hierarchal pins as you would like to see them. The d2a_converter schematic should now appear as shown below. August 15, 2012 Page 113 of 207

114 8. Choose Tools > Generate Block Symbol. 9. In the Generate Symbol dialog, click the Advanced button. 10. In the Advanced Options dialog set Pin spacing and Pin length to and click OK to return to the Generate Symbol dialog. August 15, 2012 Page 114 of 207

115 DxDesigner Tutorial for the Expedition Enterprise Flow 11. Click OK in the Generate Symbol dialog. The Symbol Editor will be launched to allow you to inspect and, if needed, change the symbol. Notice that the nets that had hierarchical ports are all represented on the symbol. Note: The exact positioning of the pins on your symbol may differ from the screenshot above. In the steps below, you will modify the position of the symbol pins. 12. Use the Pins dialog to set the V_REF pin s side to Top. August 15, 2012 Page 115 of 207

116 13. Position the V_REF pin centered on the top of the symbol. 14. Rotate the V_REF name so it can be read horizontally by selecting the pin name and clicking the Rotate 90 icon. 15. The symbol should appear as shown below. Make modifications as needed to match the symbol below. Note: If you move a pin, the pin s name will follow it. 16. Update the symbol outline by choosing Symbol > Update Symbol Outline. 17. When you have completed the symbol edits, choose File > Save All and exit the Symbol Editor. August 15, 2012 Page 116 of 207

117 DxDesigner Tutorial for the Expedition Enterprise Flow Exercise 3: Using a Hierarchical Block Now that you have created a hierarchical block for the d2a_converter, you will find symbol in the project s Local Symbols and you will be able to add this block in other schematics within the project. Each time you add the symbol, the underlying schematic will also be added. 1. Launch DxDataBook. 2. In the Navigator, double-click the systemdesign schematic under the Boards tree. 3. In DxDataBook, select the CL View and the Symbol View tab. 4. If needed, expand the width of the Symbol column so you can read the names of the symbols. August 15, 2012 Page 117 of 207

118 5. Expand the [local symbols] partition and select the d2a_converter.1 symbol. 6. Drag and drop the symbol from the preview pane into the systemdesign schematic, placing it in the location shown below. 7. Connect all of the nets and busses in that part of the schematic to the d2a_converter symbol. 8. In the schematic, click the RMB on the new symbol and choose Push from the menu. This will open the underlying d2a_converter schematic that you created. 9. Click the systemdesign tab at the top of the schematic editor to return to the top level August 15, 2012 Page 118 of 207

119 DxDesigner Tutorial for the Expedition Enterprise Flow of the design. 10. Double-click the d2a_converter symbol to invoke the Properties dialog. 11. In the Name property, enter D2A_CONVERTER in the value. Note: Now that you have added the d2a_converter block to the systemdesign board, the DxDesigner Navigator displays d2a_converter as a branch under the systemdesign board. If you look in the Blocks tree in the Navigator you will also see the d2a_converter there. These two schematics are the same. A change in one will be reflected in both. The primary difference between a schematic in the Block tree versus the Boards tree is that the Boards schematic is treated as a schematic that will be sent to Expedition PCB. Blocks, on the other hand, are treated like an element in a library. In essence, the Blocks tree can be thought of as a local library for the project. One practical difference between Blocks and Boards is that there are several commands in the Tools menu that can only be run on Boards. For example, Packager and Cross Reference operate only on Boards, not Blocks. August 15, 2012 Page 119 of 207

120 Exercise 4: Top-Down Hierarchical Design Hierarchical blocks can also be created using a top-down method. In the top-down method a block symbol is created first and the underlying schematic is created later. The top-down methodology is helpful to designers who prefer to partition a design into functional blocks prior to creating the detailed circuitry. In this exercise a top-level block will be created. The Block feature creates a symbol that resides within the project. Such symbols are called local symbols. Blocks are initially concentric rectangles where the outer boundary is sensitive to nets and busses. When a net or bus terminates at the boundary of a block, a pin is automatically added to the block. The block pins adopt the name of the nets and busses. When a block is completely defined and there is no need to add further pins it should be frozen in order to suspend the dynamic behavior where pins are automatically added. If there is a need to add pins at a later time a block can be unfrozen. The instructions below demonstrate the process of creating a hierarchical block using topdown hierarchical design. 1. In DxDesigner click the Block icon. 2. In the schematic pane LMB and drag to draw a box in the top right corner of the systemdesign schematic near the ARRANDALE_CPU block. August 15, 2012 Page 120 of 207

121 DxDesigner Tutorial for the Expedition Enterprise Flow 3. The Add Block dialog appears. Enter DDR3_SDRAM as the Block name and click OK to close the dialog. 4. Select all of the nets and busses that are between the ARRANDALE_CPU and DDR3_SDRAM blocks. Note: You could use Setup > Settings > Advanced to enable the Area Select by Overlap option. This would allow you to select the nets by drawing a box that overlaps the nets rather than completely encompassing them. August 15, 2012 Page 121 of 207

122 5. Drag the selected nets and busses to the boundary of the DDR3_SDRAM block. The nets will connect by abutment and pins will appear on the DDR3_SDRAM block symbol. The DDR3_SDRAM symbol is now complete. The steps that follow will finalize the symbol and begin the creation of the underlying schematic. 6. Click and drag the right side of the DDR3_SDRAM symbol to adjust the width of the symbol. Make sure that the net names fit within the symbol boundary. Note: If the block symbol is too short or too long you can also adjust the height by clicking and dragging the top or bottom boundary. August 15, 2012 Page 122 of 207

123 7. Right-click on the DDR3_SDRAM symbol and choose Freeze. Note: When a block is in the freeze state, the symbol will not automatically create pins and the symbol will not be resizable. If new pins need to be added, the symbol can be unfrozen by right-clicking it and choosing Unfreeze. Note: When a block symbol is not in the freeze state you should avoid copying it. Otherwise you run the risk of renaming the block s pin names. 8. Right-click on the DDR3_SDRAM block symbol and choose Edit Local Symbol. August 15, 2012 Page 123 of 207

124 9. In the Symbol Editor, select the outer rectangle of the symbol and delete it. Note: The outer rectangle serves to indicate where you can connect nets and busses while the block is in the unfrozen state. Now that the block has been frozen, you can delete the outer rectangle so the block will appear like an ordinary symbol. 10. File > Save All and exit the Symbol Editor. Note: When you return to the systemdesign schematic you will see that the outer box has been removed. August 15, 2012 Page 124 of 207

125 11. Right-click on the DDR3_SDRAM block symbol and choose Push. Note: The net segments attached to hierarchical input ports are automatically instantiated in the DDR3_SDRAM schematic. The port symbols establish the linking between the DDR3_SDRAM symbol and its schematic. At this point you would build the detailed circuitry for the DDR3_SDRAM section of the systemdesign board. However, we stop here and move on to other features of DxDesigner. 12. In DxDesigner, select Window > Close All. 13. If you do not intend to continue on to Chapter 6, close DxDesigner. End of Chapter 5 August 15, 2012 Page 125 of 207

126 DxDesigner Tutorial for the Expedition Enterprise Flow Chapter 6: Constraint Definition with CES In the DxDesigner Expedition Enterprise (EE) flow, CES is the constraint editing and management tool. CES stores actual physical parameters from Expedition PCB and signal integrity tools such that these values can be compared against constraint settings entered by designers. The constraint information can consist of component and trace clearances, routing constraints, and high speed signaling constraints. CES allows constraints to be assigned to each layer of the PCB stackup. Differential pair rules, routing schemes, and component and class rules can also be defined and managed within CES. Classes of constraints can be created to establish standardized collections of routing constraints. Classes can also be constructed in a hierarchical manner. In this editor, constraint modifications are as easy as changing properties. CES and DxDesigner cross probe between each other. Constraint passing is immediate since CES, DxDesigner, and Expedition PCB all share a common database. For design data completed up to this chapter, please go here: Chapter 6 Design Data. Note: You must first complete Chapter 1, and then copy this design data over the previous design data, for this design data to work properly. Exercise 1: Navigating CES 1. If DxDesigner is not running, launch it by double-clicking the ${DxTutorial}\DxTUT_Proj\DxTutorial.prj file. 2. Open the systemdesign schematic by double-clicking it under the Boards tree in the Navigator. 3. Launch CES by selecting Tools > Constraint Editing System or by clicking the CES icon. 4. Take a moment to read the CES Tip of the Day and then close it. Note: CES arranges design data into multiple spreadsheet tabs which include Trace & August 15, 2012 Page 126 of 207

127 DxDesigner Tutorial for the Expedition Enterprise Flow Via Properties, Clearances, Nets, and Parts. Other spreadsheets can be manually created or will appear as you interact with CES. 5. Click on each of the spreadsheet tabs and take a few moments to explore the contents of each tab. Use the scrollbars to navigate horizontally and vertically within the spreadsheet. Scrollbars Spreadsheet Since CES allows you to define a broad set of constraints it is sometimes helpful to use Display Groups to filter the spreadsheet columns to the subset which you intend to edit. Below you will learn how to use display groups. Display Group drop-down menu In particular, the Nets spreadsheet has over 70 columns, so display groups can August 15, 2012 Page 127 of 207

128 DxDesigner Tutorial for the Expedition Enterprise Flow greatly simplify the effort of defining constraints. 6. In the Nets spreadsheet, select the Display Group drop-down menu and select Net Properties. 7. Use the horizontal scrollbar and notice that there are less than 25 columns associated with the Net Properties display group. 8. Set the Display Group to Delays and Lengths. 9. Use the horizontal scrollbar and notice that there are less than 20 columns associated with the Net Properties display group. 10. Set the Display Group back to All. Since DxDesigner and CES are accessing the same database, DxDesigner can cross probe to CES. Thus, if you select a net or component in DxDesigner, that object will also be selected in CES. 11. In CES, enable cross probing by clicking the icon. When cross probing is enabled the Output window will report Cross probing server started (Port: 1). August 15, 2012 Page 128 of 207

129 12. In DxDesigner, select the bus named A_A_CHANNEL[7:0]. 13. Look at the CES window to see that the A_A_CHANNEL nets are selected. August 15, 2012 Page 129 of 207

130 14. In CES, expand the Constraint Classes tree in the Navigator and click the (All) object. By default, all nets belong to the (All) collection. Since this design is a work-inprogress, several Constraint Classes have already been defined. A Constraint Class is a collection of nets that will share a common set of constraints. CES supports a variety of constructs that allow you to organize and manage these constraints. The constructs are: Scheme A rule area. This is an area on the PCB where a set of clearances and other physical rules will be applied. In CES you set up the rules, but the actual area where the rules are applied is defined in Expedition PCB. Net Class -- A collection of nets that will have the same physical constraints, such as trace width, impedance, and clearance rules. Constraint Class A collection of nets that will have the same electrical constraints such as time of flight, overshoot, and net topology. August 15, 2012 Page 130 of 207

131 Exercise 2: Assigning Constraints and Understanding Constraint Class Hierarchies 1. In the CES Navigator expand the DDR3 constraint class. Notice that there are five other constraint classes under DDR3. This allows you to create hierarchies of constraints. Thus, a constraint that is assigned to the DDR3 level would apply to all nets assigned to DDR3 and the five underlying constraint classes. However another constraint could have different values in DDR3\DDR3_Addr versus DDR3\DDR3_Clk. If you assign a constraint at two or more levels, CES will prompt you to choose how you want the constraints to propagate to the nets. Below you will experiment with the way constraint values can be assigned and managed in CES. Note: The Actual column under # Vias is reserved to report the actual number of vias that are found in the routed Expedition PCB design. When these nets are routed, you will be able to select Data > Actuals > Import > Import Layout Actuals to compare the constraint limit to the actual number of vias found in the design. 2. In the DDR3 row of the Nets spreadsheet, enter 2 as the Max value for # Vias and press the Enter key. Notice that the value propagates down to all of the underlying constraint classes. August 15, 2012 Page 131 of 207

132 DxDesigner Tutorial for the Expedition Enterprise Flow 3. Next, enter 1 as an override value for the DDR3_Clk constraint class. 4. Go to Setup > Settings > Display > General, and change the Change Impact Dialog radio button to Always prompt user for all values. Now change the top level (DDR3) # Vias constraint to 3 and press the Enter key. 5. The Multi-Level Propagate dialog will appear allowing you to determine how to handle the propagation of this new value to the lower level constraint classes. In the dialog, read the description of each of the options. Choose Keep Overrides. August 15, 2012 Page 132 of 207

133 DxDesigner Tutorial for the Expedition Enterprise Flow 6. Experiment with this feature by assigning another value at the top level (DDR3) and choosing different propagation options. 7. When you have tried each of the propagation options, Type 3 in # Vias of the DDR3 constraint class and Discard Overrides. Exercise 3: Creating Constraint Classes In this exercise you will create a new hierarchy of constraint classes, assign nets to these classes and specify values for the associated constraints. 1. In the CES Navigator, click the RMB on the Constraint Classes tree and choose New Constraint Class. 2. A default name based on your computer s login name is given to the new constraint class. Type in a new name of AA_BB_Channel. August 15, 2012 Page 133 of 207

134 DxDesigner Tutorial for the Expedition Enterprise Flow 3. Click the RMB on the AA_BB_Channel constraint class and choose New. This creates a constraint class under AA_BB_Channel, again with a default name. 4. Type A_A_Channel as the name for this new constraint class. 5. Repeat steps 3 and 4 to create two more constraint classes under AA_BB_Channel. Name them A_B_Channel and Clk. The constraint classes should appear as shown below. 6. Click the RMB on Clk and choose Assign Nets. 7. In the Assign Nets to Constraint Class dialog, type A_CLK in the search cell and press the search button. August 15, 2012 Page 134 of 207

135 8. In the Nets in source constraint class pane, select A_CLK and press the > button to move it to the Nets in target constraint class pane. Select OK to exit the dialog. 9. Click the RMB on A_A_Channel and choose Assign Nets. 10. In the Assign Nets to Constraint Class dialog, type A_A_* in the search cell and press the search button. August 15, 2012 Page 135 of 207

136 11. Press the > button to move the A_A_Channel nets to the Nets in target constraint class pane. 12. Repeat the procedure once more to add the A_B_Channel nets to the A_B_Channel constraint class. 13. In the CES Navigator, select the AA_BB_Channel constraint class and review the Nets spreadsheet to ensure that you have the nets associated with the proper constraint classes. 14. Click any - icons under the A_A_Channel Constraint Class to show only the electrical nets in the CES spreadsheet. August 15, 2012 Page 136 of 207

137 15. The nets should appear under the constraint classes as shown below. 16. In AA_BB_Channel row of the Nets spreadsheet, set the # Vias Max to 3. Remember that you will need to press the Enter key to assign the constraint value. August 15, 2012 Page 137 of 207

138 17. Also in the AA_BB_Channel row of the Nets spreadsheet, set the External and Internal Max Restricted Layer Length to In the Clk row change the External and Internal Max Restricted Layer Length to 100. Notice that the Multi-Level Propagate dialog did not appear. This is because the Clk constraint class is the lowest level, so there are no additional levels for constraint value propagation. In other words, constraint values do not propagate upward in a hierarchy. 19. In the Nets spreadsheet scroll over to the right until you see the Type constraint under the Length or TOF Delay heading. Note: If you can t find the spreadsheet columns that you need to edit, first check to make sure you have the proper spreadsheet tab active. If you still don t see the columns you need, make sure that the Display Group is set to All. With the Type set to Length all of the other constraints under the Length or TOF Delay heading will be interpreted as physical lengths (0.001 in., since we are using August 15, 2012 Page 138 of 207

139 DxDesigner Tutorial for the Expedition Enterprise Flow English units in this tutorial). 20. If you don t see the Match constraint, scroll further to the right until you see the Match column. 21. In the Match cells for the A_A_Channel nets, set the value to A_A_Channel. You can use copy (Ctrl-C) and paste (Ctrl-V) commands to simplify the task. 22. In the Match cells for the A_B_Channel nets, set the value to A_B_Channel. The Match constraint requires that all members of a given match group have a length within the specified tolerance as defined by the Tol constraint. In the steps below you will set values for the match group tolerance. 23. Set the Tol constraint for any of the A_A_Channel nets to 50. Notice that the tolerance is applied to all other nets that are part of the match group. August 15, 2012 Page 139 of 207

140 24. Set the Tol constraint for any of the A_B_Channel nets to 50. Exercise 4: Net Classes and Schemes In this exercise you will assign the nets found in the AA_BB_Channel constraint class to a Net Class. Typically, net classes are defined by the PCB designer because the constraints associated with net classes tend to be associated with manufacturability and other physical aspects of the board. The process for creating Net Classes and Schemes is the same as the method you learned for creating Constraint Classes; therefore, we will not create new constraint classes, but simply assign nets to a Net Class. August 15, 2012 Page 140 of 207

141 1. In the CES Navigator expand the Net Classes tree. Notice that several net classes have already been defined for the design. 2. Select the All_Channels net class and inspect the associated constraints in the Trace & Via Properties spreadsheet. Notice that the trace widths and differential spacing has been set for the All_Channels net class for each routing scheme. As mentioned earlier, a scheme is a physical area on the PCB where a set of rules (constraints) and clearances apply. The PCB designer will define a polygon and assign it to one of the defined routing schemes. August 15, 2012 Page 141 of 207

142 DxDesigner Tutorial for the Expedition Enterprise Flow The default scheme is called Master and the rules associated with Master are applied to all parts of the board not otherwise associated with a defined scheme. 3. In the Trace & Via Properties spreadsheet, expand the All_Channels tree under the Master scheme. Note: Further detail is revealed allowing you define constraints for each layer of the board stackup. A check mark in the Route column indicates that the layer allows unrestricted routing. Layers without a check mark are subject to the Max Restricted Layer Length constraint that we defined in the Nets spreadsheet earlier in this chapter. 4. Expand the BGA scheme and the All_Channels net class. August 15, 2012 Page 142 of 207

143 DxDesigner Tutorial for the Expedition Enterprise Flow Note: The top-level trace width (th) is 10 thousandths, yet this value has been overridden on most of the layers where the constraint is actually 4 thousandths. One would think that under a BGA, the trace width rules would be equal or smaller than the default settings, so the value of 10 th seems a bit odd. For now, we ll trust that there is a reason for these settings, but if you found such a rule in an actual design, it would be a good idea to visit the author of the constraint to verify that it is accurate. So, what do all of these rules mean? Consider an example involving the nets that belong to the All_Channels Net Class. Anywhere on the board that is not governed by a defined scheme, the trace widths for the Master scheme apply. Thus, All_Channels nets will have a typical trace width of 4 th. If an All_Channels net enters a region where the scheme BGA exists, the trace width will depend on the board layer. If the net is on layer SIGNAL_1 the typical trace width would also be 4 th. However, if the net traveled through the BGA area on layer SIGNAL_10, the typical trace width would be 10 th. Once the trace exits the BGA scheme region, the trace width rules would revert to the constraints defined by Master (presuming the trace did not enter a region controlled by a different scheme). Now that you have inspected the All_Channels Net Class, you will assign the A_A_Channel and A_B_Channel nets to it. 5. Activate the Nets spreadsheet. 6. Scroll the view to the left until you view the Net Class column. August 15, 2012 Page 143 of 207

144 7. At the A_A_Channel row, set the Net Class constraint to All_Channels. 8. The Multi-Level Propagate dialog will appear. Click Discard Overrides to propagate the net class to all of the nets under A_A_Channel. 9. Use the same method to assign All_Channels to the A_B_Channel nets. 10. For now leave the Clk constraint class in the Default net class. Close CES. End of Chapter 6 August 15, 2012 Page 144 of 207

145 DxDesigner Tutorial for the Expedition Enterprise Flow Chapter 7: Preparing a Schematic for PCB Design This exercise will walk you through the process of verifying your DxDesigner schematic and sending it to Expedition PCB. First you will run the DxDesigner Diagnostics to ensure the integrity of the schematic database. The two primary methods for verifying a design are DxDataBook and Tools > Verify. You will use DxDataBook s Hierarchical Verification feature to confirm that every part in the schematic has all of the required properties. Then, Tools > Verify will perform both syntax and design rule checks. Finally, you will run the Packager to prepare the schematic data for placement and routing in Expedition PCB. The Packager will check to confirm that the all symbols have a corresponding part definition in the Central Library and that all parts have pin numbers and a unique reference designator. If the schematic fails any of the checks performed by Packager, errors will be recorded in Partpkg.log in the Logfiles directory of the open project. The design will not open in Expedition PCB until Packager is able to be run without errors. For design data completed up to this chapter, please go here: Chapter 7 Design Data. Note: You must first complete Chapter 1, and then copy this design data over the previous design data, for this design data to work properly. Exercise 1: DxDesigner Diagnostics DxDesigner Diagnostics are a series of tests that can be run on a schematic to determine if there are any issues with the schematic database. If a problem is found, the diagnostics can also be used to make corrections to the schematic. 1. If DxDesigner is not running, open the DxTutorial project by double clicking the ${DxTutorial}\DxTUT_PROJ\DxTutorial.prj file. 2. In the DxDesigner Navigator, double-click on the systemdesign board to open the top-level schematic. August 15, 2012 Page 145 of 207

146 3. Select Tools > DxDesigner Diagnostics. The Output pane will open a tab named DxDesigner Diagnostics and record the results of each test as it is run. When the diagnostics have completed, a summary will be provided detailing how many tests were run and how many of them passed. In the screenshot below, notice that 17 tests passed and one test failed. 4. In the Output pane, review the results of your diagnostics. If you had any errors, scroll upward to see what diagnostics failed. If a diagnostic failed, the Output pane would report which diagnostic failed along with the location of the failure. $1N184 August 15, 2012 Page 146 of 207

147 5. If you had any diagnostic failures, scroll to the bottom of the diagnostics summary and click the link named Click here to fix all errors. When the diagnostic fixes are applied, the Output pane will report the results of the corrections. Note: If you had to fix any errors, it is a good practice to run the diagnostics a final time to ensure that all diagnostics have passed. In the DxDesigner Diagnostics tab of the Output pane, click the RMB and choose Clear to flush your previous diagnostic reports. August 15, 2012 Page 147 of 207

148 6. If you ran Diagnostics to fix any errors, right-click in the Output pane and choose Clear and then select Tools > DxDesigner Diagnostics to ensure that all diagnostics have passed. If you want to have DxDesigner Diagnostics run each time you switch projects or close DxDesigner you can configure DxDesigner to do just that. The steps below will show you how to configure this feature. 7. In DxDesigner select Setup > Settings > DxDesigner Diagnostics. August 15, 2012 Page 148 of 207

149 8. OPTIONAL: Enable the Execute DxDesigner Diagnostics on exit option. Note: It is not required that you enable diagnostics to run on exit, but it might be a good idea to try using this mode for the balance of this tutorial. 9. Click OK to close the Settings dialog. Exercise 2: Hierarchical Verification with DxDataBook Earlier in this tutorial you performed Live Verification with DxDataBook to confirm that a few parts on a schematic sheet had a matching component in the DxDataBook database. We ll follow a similar series of steps to perform Hierarchical Verification which has the ability to verify all parts in a schematic. One notable difference between Hierarchical and Live Verification is that Hierarchical Verification will store any component changes into a queue called the Pending List. When you want to apply component changes to your schematic you will execute an operation that applies all updates in the Pending List. Otherwise, the Hierarchical Verification and Live Verification processes are very similar. 1. In the DxDesigner Navigator, double-click the systemdesign board to ensure that DxDataBook will verify the entire systemdesign hierarchy. 2. Close the Output window to make room for DxDataBook. 3. Invoke DxDataBook. August 15, 2012 Page 149 of 207

150 DxDesigner Tutorial for the Expedition Enterprise Flow 4. In DxDataBook, invoke a New Hierarchical Verification Window. 5. In DxDataBook, click the green exclamation mark to execute the verification on the systemdesign schematic. August 15, 2012 Page 150 of 207

151 During Hierarchical Verification, DxDataBook will evaluate all parts on all sheets and all levels of a schematic in an attempt to find matching parts in the DxDataBook database. As you saw earlier in the tutorial, the results will be flagged by a colorcoded circle (red, yellow, green). However, there is result that you have not yet seen: the question mark (? ) indicates that a symbol was not found at all in the database. Typically, this result will occur with local symbols symbols which have been created within the project and are not part of the DxDataBook library. For example, the d2a_converter symbol that you created in Chapter 5 will have a status of Cannot Find Library. In the case of the systemdesign schematic, there are several hierarchical blocks that are used to partition the design into meaningful sections. These symbols are not part of the DxDataBook database and are therefore tagged with the? code. 6. Inspect the list of these parts that have the? code. Notice that most are hierarchical blocks, yet some are also an FPGA circuit that apparently is not part of the DxDataBook library. August 15, 2012 Page 151 of 207

152 7. Scroll downward to review the remaining parts in the design. Note: You should find that all but four of the other parts are tagged with the green code which means an exact match was found in the DxDataBook database. Depending on how you followed the instructions in the earlier chapters, you may have different results from the hierarchical verification. Clicking on the match indicator column header will order the matches according to color. 8. Click the RMB on the yellow-coded capacitor and choose Visit by name and select any of the names from the list that appears. August 15, 2012 Page 152 of 207

153 9. Inspect the schematic sheet where these capacitors appear. 10. In the DxDataBook pane, double-click the part tagged with the yellow Missing Properties code. 11. In the middle pane of DxDataBook you should see only one match in the search list. Select that row and click the Add Part to Pending List icon. August 15, 2012 Page 153 of 207

154 12. Click the Update Design icon at the top of the DxDataBook dialog. Note: In the verification results pane the capacitor is now tagged as OK After Update. 13. Sort the Status column and confirm that all parts now have either OK or Cannot Find Library as the status. Note: You should now have three types of resistors that are failing the verification by DxDataBook. These failing resistors are the ones on which you changed the Tolerance during Chapter Double-click the row that corresponds to resistor R In the middle pane of DxDataBook, right-click on the Tolerance column and choose Remove Condition. Note: A single resistor is now visible in the middle pane. August 15, 2012 Page 154 of 207

155 DxDesigner Tutorial for the Expedition Enterprise Flow 17. In the middle pane, select the row corresponding to Part Number and click the Add Part to Pending List icon. 18. Follow the same process outlined in steps 15 through 17 to add the other two resistor types to the Pending List. 19. When all three resistor types have the OK After Update status, click the Update Design icon. 20. If you have any other parts tagged with the yellow or red indicator, use the methods you ve learned to correct those parts now. 21. Close the DxDataBook pane. Exercise 3: Design Rule Checks with Tools > Verify DxDesigner provides an integrated and customizable design rule checker. The Verify utility will evaluate a wide range of electrical, HDL, and syntactical issues with your schematic. Given that hardly any two design flows are exactly alike, the tests that Verify can perform can be customized to your unique tool flow needs. In this exercise you will configure and execute some design rule checks on the systemdesign schematic. 1. In the DxDesigner Navigator, select the systemdesign board to set the focus of DxDesigner to the top level of the board. 2. In DxDesigner select Tools > Verify. 3. Note that the banner of the DRC dialog confirms that the scope of the verification is the systemdesign schematic. Make sure the Check option is set to Board. August 15, 2012 Page 155 of 207

156 DxDesigner Tutorial for the Expedition Enterprise Flow 4. Click the Rules tab. 5. Click on any one of the tests and notice that a description of the test is provided at the bottom of the DRC dialog. 6. Scroll down through the list of tests to familiarize yourself with the tests. The tests that Verify performs are organized into nine groups: Migration: syntax checks, legal characters, name and property lengths Connectivity: hierarchical and flat connectivity checks Electrical: checks for pull-ups/pull-downs, polarity checks Hierarchy: checks to ensure hierarchical connectivity Integrity: missing properties, pin number checks Power&Ground: floating supply pins, legal global signals, implicit /explicit power Device Specific: ICs, bus transceivers, op amp checks HDL Checks: Verilog and VHDL keywords, VHDL data type and model availability Links: tests integrity of link objects in the schematic Design rule checks can be enabled either as entire groups or as individual checks. Checkboxes in the Rules tab are used to enable a specific group or test. The Rules tab also allows you to configure settings/limits for each test along with the severity of the associated error message. August 15, 2012 Page 156 of 207

157 DxDesigner Tutorial for the Expedition Enterprise Flow 7. In the Rules tab, enable the Migration group. This enables each of the individual tests under Migration Group. 8. Deselect drc-004. August 15, 2012 Page 157 of 207

158 DxDesigner Tutorial for the Expedition Enterprise Flow 9. Click OK to execute the tests. 10. Review the DRC output messages. Note: You will see that 26 drc-002 errors occurred and two drc-006 errors occurred. The drc-002 errors are caused by net name characters that Verify considers illegal. The drc-006 errors are caused by two symbols having a property named RB Layer Map which exceeds the 80 character limit on property values. You will first focus on correcting the drc-002 errors. If you look at the net names that failed drc-002 you might guess that this check is failing on the $ and ~ characters. If you add these characters to the parameters for drc-002 you should be able to clear this error. Note: Editing parameters for Verify really should be the job of a tools administrator and/or a librarian. Schematic designers ought to avoid making changes to the rules for Verify. If a test failed and you felt that it may be an erroneous result, you should discuss it with your tools administrator. 11. In the DRC tab of the Output pane, right-click and choose Clear. 12. Select Tools > Verify to launch the DRC dialog and activate the Rules tab. 13. Inspect the Values cell associated with drc-002. August 15, 2012 Page 158 of 207

159 14. Change the Values for drc-002 to read as follows: ^([a-za-z_ ~$]*)$ Note: This format makes the $ and the ~ characters acceptable to drc-002 regardless of where in the string these characters appear. 15. Click OK to run the design rule checks again. Note: Now only the two drc-006 errors occur. This test checks the length of property values and will issue an error if a property s value exceeds a limit that is defined in the Rules tab. 16. In the DRC tab of the Output pane, RMB > Clear. 17. Open the DRC dialog (Tools > Verify). 18. Change the value for drc-006 to 255. August 15, 2012 Page 159 of 207

160 DxDesigner Tutorial for the Expedition Enterprise Flow 19. Click OK to execute the tests with the new settings. The tests should complete with 0 errors. Exercise 4: Packager The Packager will prepare the schematic database for the place and route phases that will be completed in Expedition PCB. Packager will assign reference designators and pin numbers where needed. For each part in the design, Packager will make a local part database. This process ensures that each part in the schematic is properly represented in the Central Library. If there are duplicate reference designators or parts missing in the Central Library, Packager will issue error messages. If you receive any error messages, they must be resolved prior to your being able to open the design in Expedition PCB. In this exercise you will run Packager on the systemdesign schematic. 1. In DxDesigner select Tools > Package. Note: Any Errors, Warnings, or Notes that occur are recorded in the Partpkg.log file in the \logfiles folder of the project. It is a good practice to review the Partpkg.log file after running the Packager. August 15, 2012 Page 160 of 207

161 2. Configure the settings as shown below and click OK to execute the Packager on the systemdesign board. August 15, 2012 Page 161 of 207

162 DxDesigner Tutorial for the Expedition Enterprise Flow 3. Packager messages will be recorded in the Packager tab of the Output pane. If the packaging was successful, the Output pane will report the message shown below. For normal operation, the options shown here should be sufficient for packaging your designs. The Packaging Options can be configured such that the Packager will remove all pre-existing reference designators and assign new ones. This is an operation that you must be careful to use only when it is appropriate. Similarly, the PDB Extraction Options can be configured to control the operation where part data is fetched from the Central Library and stored locally in the project. If your Central Library has changed, you may need to use one of the options that would delete and rebuild the local library. Note: Caution must be used when selecting Repackage All Symbols from the Operation drop-down in the Packaging Options section of the Packaging Dialog as this option will remove all pre-existing reference designators and assign new ones. More details on these options are provided in the DxDesigner documentation as well as in Mentor Graphics DxDesigner courses. August 15, 2012 Page 162 of 207

163 Exercise 5: Expedition PCB During this exercise you will open the systemdesign board in Expedition PCB and explore some of the basic features of Expedition PCB. You will import your design into Expedition PCB, place some parts, renumber reference designators, and back annotate your changes to the schematic. The Following video will give you a brief overview of some of those techniques. Video: Create a PCB with Expedition Enterprise (5 min). In Chapter 4 you added the Cluster property to the components in the d2a_converter schematic. The Cluster property enables the PCB designer to identify and tightly group components sharing this property in Expedition. This exercise will demonstrate the advantage of using the Cluster Property. 1. In DxDesigner, select Tools > Expedition PCB or click the Expedition PCB icon. Where this is the first time schematic data is being passed forward to Expedition layout you need to select a layout Template using the Select Template drop-down in the DxDesigner To Expedition PCB dialog to choose the desired Template as shown below. PCB templates can be thought of as seed boards. They can be as simple as a bare board outline or they can be boards that are partially placed and routed. The test template, as you will see, is partially placed and routed. Note: The PCB directory setting may differ from the screenshot if you installed the tutorial data in a location other than c:\. August 15, 2012 Page 163 of 207

164 DxDesigner Tutorial for the Expedition Enterprise Flow 2. Use the Select template drop-down menu to select the systemdesign template. 3. Accept the default PCB directory setting and click OK. Note: The DX2EXP dialog will inform you that the PCB directory does not exist. 4. Click OK to the warning about the target design having 12 metallic layers. 5. Click OK to create the new directory for the PCB design. August 15, 2012 Page 164 of 207

165 6. Note: When Expedition PCB is invoked, you may need to bring the Expedition layout window to the foreground on your screen. After doing so, you will see a dialog requesting confirmation that you wish to forward annotate DxDesigner data to Expedition. 7. Forward Annotating to Expedition PCB reads the schematic data and imports any changes that were made to the schematic since the last time you forward annotated data to Expedition. 8. When Expedition PCB invokes, click Yes to Forward Annotate the design. 9. The template board will appear along with the Project Integration dialog. The Project Integration dialog allows you to control how unused parts and traces are handled if symbols and nets have been removed from the schematic. Additionally, Forward Annotation will cause new symbols and nets to be added to the PCB database. August 15, 2012 Page 165 of 207

166 DxDesigner Tutorial for the Expedition Enterprise Flow 10. Set the Library extraction options to Delete local data; then rebuild all local library data. This will ensure that all part details are up to date with the Central Library. August 15, 2012 Page 166 of 207

167 11. In the Project Integration dialog, click the amber button named Forward Annotation Required, connectivity changed. 12. When the Forward Annotation is complete, notice that the pending schematic CES changes were also updated in the PCB database and all status indicators are now green. 13. Close the Project Integration dialog. Note: In Chapter 4 you created the d2a_interface schematic. At that time you added the Cluster property to each of the parts. In the following steps you will use the Cluster property for placing these parts. 14. In Expedition PCB, select Place > Place Parts and Cells. 15. If the Reusable Block License Requirement dialog appears, click OK Note: This board has a pair of reusable blocks. In DxDesigner, an advanced license is required to place reusable blocks. In this exercise, you will not interact with the reusable blocks so it will not matter whether or not you own that license. August 15, 2012 Page 167 of 207

168 DxDesigner Tutorial for the Expedition Enterprise Flow 16. In the Place Parts and Cells dialog, make sure the Unplaced and Placed options are checked and the other Include options are unchecked. 17. Use the Criterion drop-down menu to choose Cluster. Note: The DA_Converter cluster that you created appears in the list of cluster names. Note that the # column specifies how many parts are in the cluster. There are six parts because when you created a copy of the D2A circuit, the Cluster property was also copied. 18. Select the DA_Converter cluster name. 19. Click the single downward pointing arrow to load the DA_Converter cluster for placement. August 15, 2012 Page 168 of 207

169 DxDesigner Tutorial for the Expedition Enterprise Flow 20. Use the Action drop-down menu to select Place and ensure that Method is set to Sequence. Note: When you click Apply, the parts in this cluster attach to your cursor in sequence for placement in Expedition. August 15, 2012 Page 169 of 207

170 21. In the list of Active Parts, select RefDes IC Use the Active angle drop-down menu to change the option to 90 degrees. August 15, 2012 Page 170 of 207

171 DxDesigner Tutorial for the Expedition Enterprise Flow 23. Click Apply. 24. The Place Parts and Cells dialog will temporarily disappear and the focus of the mouse cursor will move to the Expedition PCB window. Note: You can roll the mouse wheel to zoom in and out of the board view. 25. Position IC1 on the left side of the board and press the LMB to place the cell in the location shown below. IC1 Note: When you placed IC1, the list of Active parts displays a P meaning placed next to the RefDes column. August 15, 2012 Page 171 of 207

172 26. Repeat the process to add IC2 to the right of IC1. IC2 27. In the Place Parts and Cells dialog, change the Active Layer setting to Bottom. 28. Select C52 and click Apply and place it underneath IC Select C54 and click Apply and place it also below IC1. August 15, 2012 Page 172 of 207

173 DxDesigner Tutorial for the Expedition Enterprise Flow 30. Use the same process to place C53 and C55 beneath IC The DA_Converter parts should appear as shown below. 32. Close the Place Parts and Cells dialog. 33. In Expedition PCB, select ECO > Renumber Ref Des. August 15, 2012 Page 173 of 207

174 DxDesigner Tutorial for the Expedition Enterprise Flow 34. In the Process list, assign IC1 a new Ref Des of IC Assign IC2 a new Ref Des of IC Click Apply to change the Ref Des properties. 37. In the graphic area of the Renumber Reference Designators dialog, pause the mouse cursor over each of the DA_Converter ICs to see that the Ref Designators have been changed. August 15, 2012 Page 174 of 207

175 DxDesigner Tutorial for the Expedition Enterprise Flow 38. Close the Renumber Reference Designators dialog. 39. In Expedition PCB, select Setup > Project Integration. Note: The Project Integration dialog now indicates that back annotation is required. At this time, the new Ref Designator values in Expedition have not yet been updated in DxDesigner. 40. In the Project Integration dialog click the Additional Options button. August 15, 2012 Page 175 of 207

176 DxDesigner Tutorial for the Expedition Enterprise Flow 41. Enable all of the check boxes in the Additional Options dialog. Note: The Create eexp View during Back Annotation option will create the files necessary for viewing the PCB layout while you are working in DxDesigner. 42. Click the amber button labeled Back Annotation Required. 43. When the Back Annotation indicator becomes green, close the Project Integration dialog. 44. Close Expedition PCB. 45. In DxDesigner, select the d2a_converter in the schematic and push into it. August 15, 2012 Page 176 of 207

177 DxDesigner Tutorial for the Expedition Enterprise Flow 46. Inspect the Ref Designator properties on the ICs to ensure they are now IC100 and IC200. Exercise 6: eexp View The eexp View feature in DxDesigner allows you to view the Expedition PCB layout within the DxDesigner window. The DxDesigner editor and the eexp View window will cross probe. The eexp View relies on a CCZ file of the PCB layout which is generated by Expedition PCB. CAMCAD CC / CCZ files are the ASCII XML intelligent hierarchical files becoming a standard in the EDA realm. The CC file structure allows for archiving and neutralizing data from all industry popular Vector Graphics formats, Intelligent PCB Layout formats, and EDIF Schematic 200 & 300 formats, giving engineers unprecedented access to all the information in a single ASCII XML format. CCZ files are compressed CC files, using standard PKZip/Winzip compression. The advantage of using DxDesigner s eexp View is that a schematic designer does not have to consume an Expedition PCB license to view the PCB layout. Note: The CCZ file is a snapshot of the Expedition PCB layout. Therefore, if a change is made in Expedition PCB, the changes to the layout will not be seen by eexp View until back annotation has been performed. August 15, 2012 Page 177 of 207

178 1. In DxDesigner, select View > eexp View. Note: The eexp View pane will appear at the bottom of the DxDesigner window. August 15, 2012 Page 178 of 207

179 DxDesigner Tutorial for the Expedition Enterprise Flow 2. In the eexp View pane, roll the mouse wheel forward to zoom in on the DA_Converter parts that you placed on the board. 3. In the eexp View pane, click on IC100. Note: Selections made in the eexp View pane cross probe to the schematic editor. August 15, 2012 Page 179 of 207

180 4. In the DxDesigner schematic editor, select IC200. Note: Selections made in the schematic editor will cross probe to the eexp View pane. 5. In the eexp View pane, right-click and choose Show/Hide Toolbar. August 15, 2012 Page 180 of 207

181 DxDesigner Tutorial for the Expedition Enterprise Flow 6. Take some time to experiment and become familiar with the toolbar icons in eexp View. 7. In DxDesigner, select Window > Close All. 8. If you do not intend to continue on to Chapter 8, close DxDesigner. End of Chapter 7 August 15, 2012 Page 181 of 207

182 DxDesigner Tutorial for the Expedition Enterprise Flow Chapter 8: Documenting DxDesigner Schematics DxDesigner has several utilities that support the documentation of a schematic including Cross Reference, DxPDF, Partlister and Archiver. Cross Reference adds properties to the schematic that make it easy to trace a net through the schematic. DxPDF produces an intelligent PDF document from the schematic that has several features that would be helpful to colleagues and vendors who do not have access to DxDesigner. The Partlister can create both part lists and other reports that list any of the properties on your schematic symbols. Lastly, Archiver saves a copy of all of the relevant project files to a location of your choice. In this chapter you will learn how to use each of the above utilities and you will become familiar with their optional configurations. For design data completed up to this chapter, please go here: Chapter 2 Design Data. Note: You must first complete Chapter 1, and then copy this design data over the previous design data, for this design data to work properly. Exercise 1: Cross Referencing The Cross Reference utility annotates properties to on-sheet and off-sheet pins as well as to hierarchical blocks in order to help designers trace nets throughout the schematic. Cross reference properties are especially helpful to designers who are working with a printed copy of the schematic. In this exercise you will annotate the systemdesign schematic with cross reference information. Nets that have Link symbols will be cross referenced. Additionally, hierarchical blocks will be annotated with a SHEET property that report which schematic sheets reside below the block. Cross Reference Settings Cross Reference requires that all schematic sheets are closed prior to running the cross referencing operation. This is because Cross Reference annotates a schematic in two phases: the record phase and the place phase. During the record phase, Cross Reference traverses the schematic to determine what cross references will be written. During the place phase, Cross Reference writes the annotations to the components in the August 15, 2012 Page 182 of 207

183 DxDesigner Tutorial for the Expedition Enterprise Flow schematic. Therefore, Cross Reference has to ensure that no changes occur in the schematic between the record and place phases. All settings for Cross Reference are contained in scout.ini file. The scout.ini file is an ASCII text file that is copied into the project directory when Cross Reference is run or the settings are modified. In the steps below, you will modify the settings for Cross Reference using a dialog, but it is worthwhile to understand that these settings could also be configured using a text editor. 1. If DxDesigner is not running, open the DxTutorial project by double clicking the ${DxTutorial}\DxTUT_PROJ\DxTutorial.prj file. 2. If any schematics are open, close all schematic sheets by selecting Window > Close All. 3. Select Tools > Cross Reference to launch the Cross Reference dialog. Note: The Top Level Block is set to systemdesign. Cross Reference is one of the utilities that only operate on Boards and not the Blocks section. If you selected the drop-down menu, you would only see the Boards that are associated with this project. August 15, 2012 Page 183 of 207

184 4. In the Introduction page of the Cross Reference dialog, select Modify Cross Reference Settings and click Next. Note: If you had already run Cross Reference on your schematic, it would be important to FIRST use the Remove Cross References Using Existing Settings option before you make any changes to your Cross Reference settings. If you failed to remove pre-existing cross references, you may find that you have old cross references cluttering your schematic. 5. Click Next again to display the Cross References Options page. record place August 15, 2012 Page 184 of 207

185 Note: The cross reference property will be named XREF. The Format Entry option is configured such that the XREF property is written in the format of a page number followed by a vertical and horizontal zone name (e.g., 2-C5). The several pin symbols shown are pre-configured to be cross referenced. Each pin symbol has two entries. The entry without the Annotation options will create a record command in the scout.ini file. The entry with the Annotation options will create a place command in the scout.ini. If you add a new pin symbol to the scout.ini file it is vital that you create both record and place commands. The hier_in.1 pin has been left out of the scout.ini file. In the following steps you will add the required two rows in order to have Scout cross reference the hier_in.1 pin symbols. 6. Right click anywhere in the Record and Place Options area and choose New Row. August 15, 2012 Page 185 of 207

186 DxDesigner Tutorial for the Expedition Enterprise Flow 8. In the new row, configure a record command by entering the following options: a. Block: Any b. Selection Type: Symbol Name c. Selection Qualifier: hier_in.1 d. Right click in the Options area again and choose New Row. e. In the new row, configure a place command by entering the following options: i. Block: Any ii. Selection Type: Symbol Name iii. Selection Qualifier: hier_in.1 iv. Annotation Point X: v. Annotation Point Y: vi. Text Origin: Middle Right August 15, 2012 Page 186 of 207

187 9. Change all cells under the Block Type column to Any. Note: The Block Type allows you to specify that Scout must find a symbol that matches both the name in the scout.ini file and the specified block type (where the Block Type can be Composite, Module, Primitive, Annotate or Pin). The Any option eliminates this added level of filtering, making it easier for Scout to annotate the symbols that you intend to be annotated. August 15, 2012 Page 187 of 207

188 10. Click Next. Note: The Direct Reference Options page configures cross reference properties that can be added to hierarchical components. In this case, directref0 is configured to put a property named SHEET onto any hierarchical (composite) symbol. The format of the SHEET property will be the range of page numbers that are below the hierarchical block. 11. Click Next to advance to the Sheet Options dialog. August 15, 2012 Page 188 of 207

189 12. On the Sheet Options dialog, the names for the horizontal and vertical zones are incorrect. For the dsheet.1 symbol that you are using, the horizontal zones are numbers and the vertical zones are letters. Use the cut/paste commands to swap the zone names so they appear as shown below. 13. Change the Zones Order Horizontal to Right To Left. August 15, 2012 Page 189 of 207

190 14. Change the Zones Order Vertical to Bottom To Top. Note: The settings for the sheet are being configured globally. Thus, any sheet border in your library would use these settings. The librarian who creates the sheet borders should be consistent in the way the zones are named. Note: The D-size sheet border you are using is divided into 8 horizontal zones and 4 vertical zones. Therefore, the vertical and horizontal distances between zones need to be adjusted. August 15, 2012 Page 190 of 207

191 15. Change the Distance Between Zones to 4.25 and 5.75, X and Y zone sizes, respectively. The zone distances should appear as shown below. August 15, 2012 Page 191 of 207

192 16. Click Next and then Finish to save the changes to the scout.ini file in your project directory. Below is an excerpt of the scout.ini file showing the edits you made to the sheet options. Note: In the scout.ini file the pipe ( ) character is a comment character. All text to the right of the pipe character is ignored by Scout. 17. Select Tools > Cross Reference again. Note: Remember that all schematic sheets need to be closed when you run Scout. 18. Select the Generate Cross References Using Existing Settings option and click Finish to execute the cross referencing operation. Note: When Cross Reference has completed, the Output pane will report: Finished scout.exe. 19. Open the systemdesign schematic. August 15, 2012 Page 192 of 207

193 20. Double-click the ARRANDALE_CPU symbol to inspect the properties. Note: The SHEET property should be a range of 7 sheets. Depending on how you created your schematic, you may find that the exact SHEET numbers differ from the screenshots below. The key thing for this exercise is that there are 7 sheets recorded by the SHEET property on the ARRANDALE_CPU block. The symbol now has a SHEET property with a value of Push into the d2a_converter block. August 15, 2012 Page 193 of 207

194 22. Zoom in on the CLK input pin and make note of the new XREF property. Note: Here again, the sheet numbers may differ from the examples shown in the screenshots. The key point is that the cross referencing is correct regardless of the sheet numbers that Scout assigned. 23. Return to the systemdesign schematic and click on the CHANNEL_OUT block. Notice that the SHEET property on this block matches the XREF you saw on the CLK signal. August 15, 2012 Page 194 of 207

195 DxDesigner Tutorial for the Expedition Enterprise Flow 24. Push into the CHANNEL_OUT block and find the CLK signal pin. Note: XREF properties can be moved manually, but the best approach would be to configure both your pin symbols and the scout.ini file such that the XREF property is created in a location that makes it easy to read. 25. Zoom out to confirm that the zone coordinates that you saw in the d2a_converter schematic are accurate. Note: The zone coordinates are based on the position of the pin to which the XREF is attached. So the zones referenced in your schematic may differ from the screenshots shown above. 26. If you find the Output pane reporting any Duplicate IDs errors (Error 1296), run Tools > DxDesigner Diagnostics and click the Fix all errors link. Exercise 2: DxPDF The DxPDF utility allows you to communicate effectively through an advanced PDF document which can be opened and viewed using the free Adobe Reader. By generating an intelligent PDF file, you can send a single file to anyone, anywhere in the world, and provide them with the ability to perform a complete design review using Adobe Reader. The PDF file created by DxPDF not only contains the graphical data of the main schematic, but it also contains hierarchical data. The PDF file can also include net and part information with symbol names and a complete list of property names and values assigned to those symbols. This functionality allows you to easily locate nets or parts using advanced search features. These advanced features include net name hyperlinks that allow you to easily trace a net throughout the schematic. Attributes can be reviewed by placing the cursor over a part, clicking the left mouse button and selecting the pop-up with the list of attributes for the part. August 15, 2012 Page 195 of 207

196 DxDesigner Tutorial for the Expedition Enterprise Flow 1. Select File > Export > PDF 2. In the Range section of the DxPDF dialog, select Block and choose systemdesign from the drop-down list. Note: The Project range option will export all boards and all blocks to the PDF file. If you choose this option, the PDF file will have duplicate sheets because some sheets appear under both the Project tree and the Blocks tree. Typically, you will want to choose the Block option so you can export only the board to the PDF file. August 15, 2012 Page 196 of 207

197 3. In the Options section of the DxPDF dialog, enable only the Start PDF Reader After Generation option. 4. Click OK to execute the PDF file generation. The PDF file will open and appear as shown below. August 15, 2012 Page 197 of 207

198 DxDesigner Tutorial for the Expedition Enterprise Flow The PDF file is stored in the project directory (the same location where you find the.prj file). The Bookmarks pane on the left lists each of the sheets in the schematic. The bookmarks are arranged in a tree according to the hierarchical structure of the schematic. 5. In the Bookmarks pane, click on the ARRANDALE_CPU Sheet 1 bookmark. Notice the viewing pane displays the sheet that you selected. 6. Click in the graphical pane of the PDF document. 7. Use the Page Down key to move to the other sheets in the ARRANDALE_CPU schematic. Note: Clicking in the graphical pane of the PDF file puts the focus of the Page Up/Page Down keys on the individual sheets. 8. Close the PDF file. 9. In DxDesigner, Launch DxPDF again by choosing File > Export > PDF. 10. Again, select the systemdesign block. 11. Enable the Add popup menu on components and Visible Component/Net Hyperlinks options. 12. Click OK to generate a new PDF file. August 15, 2012 Page 198 of 207

199 DxDesigner Tutorial for the Expedition Enterprise Flow 13. In the viewing pane of the PDF file, click on the ARRANDALE_CPU block and select Push Schematic. 14. In sheet 1 of the ARRANDALE_CPU, click some of the components and choose Properties. Note: A popup window appears which displays the properties of the selected part. In this way, the DxPDF output behaves like a view-only version of DxDesigner. 15. In Adobe Reader, select Edit > Find and enter 6.8pF in the search field. Press Enter to execute the search. Adobe Reader will navigate to the first 6.8pF capacitor that if finds. August 15, 2012 Page 199 of 207

200 16. In Adobe Reader, click the Find Next button to search for the other 6.8pF capacitor in the schematic. 17. Close Adobe Reader. Exercise 3: Partlister The Partlister generates reports that tabulate symbol properties. This is typically used for Bill of Materials (BOM) reports, but depending on the properties on your symbols, you can use Partlister to generate a wide range of helpful reports. 1. Select Tools > Partlister. The Configuration file listed in this dialog is where all of the part list settings will be stored. Your design environment could have several different.ipl files to allow you to produce a variety of reports: BOMs, cost reports, component height reports, etc. The partlister is limited only to the properties on the instantiated components on your schematic. 2. Confirm that the Scope is set to Board and that the Output format is set to Text File. August 15, 2012 Page 200 of 207

201 3. Click the Columns tab. The Columns tab lists the columns that will appear in the part list. Additionally, this tab provides controls for configuring the format of each of the columns. Below you will add a new column to the report. 4. Above the list of properties, click the New icon. August 15, 2012 Page 201 of 207

202 5. Rename the new column to Value. 6. Configure the settings for the Value property as shown below. August 15, 2012 Page 202 of 207

203 DxDesigner Tutorial for the Expedition Enterprise Flow 7. Click OK to generate the part list. Below is an excerpt of the report that will be generated. Some designers prefer not to have the reference designators compressed as shown above. Thus, where you see R76-R78 on line 20, it may be preferable to see R76,R77,R78. Below you will re-configure the Ref Designator column to list each reference designator. 8. Close the part list file. 9. Open the Partlister (Tools > Partlister) and activate the Columns tab. August 15, 2012 Page 203 of 207

204 10. In the list of Columns, select Ref Designator and set the Display Mode to Full. 11. Click OK to generate a new part list. You will now see that row 4 has many reference designators listed explicitly. 12. After you have reviewed the report, close it. August 15, 2012 Page 204 of 207

205 DxDesigner Tutorial for the Expedition Enterprise Flow Exercise 4: Archiving Projects DxArchiver is a utility that will store your project in a directory of your choice. Additionally, DxArchiver can create a PDF file of your schematic and/or compress the archive. 1. Select Tools > Archiver to launch DxArchiver. 2. Ensure the Target directory is set to..\arch 3. Ensure the Compress using zip format option is enabled. 4. Click Next > to proceed to the next page of DxArchiver. The Additional Files page allows you to add non-project files and folders to be included in the archive. In this exercise we will not add any additional files. 5. Click Finish to create the archive of your project. August 15, 2012 Page 205 of 207

206 6. Close DxArchiver upon completion. 7. Use a file browser to navigate to the \DxWDIR\DxTUTORIAL\ARCH directory and inspect the archive that was created. A.zip file and a manifest.xml file will reside in the archive directory. Note: The zip file name contains a time stamp, so the exact name of your zipped archive will differ from the one shown in the screenshot above. 8. Close DxDesigner. End of Chapter 8 August 15, 2012 Page 206 of 207